Engineering Plastics

Plastics are easy to underestimate. Pick the wrong one and you get warped parts, blown tolerances, and a customer who won't reorder. Pick right and you get parts that are lighter, quieter, and cheaper than metal equivalents. This page covers the plastics we actually machine regularly — not a textbook dump of every polymer that exists.

Which Plastic Do You Need?

Start here. Most plastic machining jobs fall into one of these scenarios.

Your Situation	Use This	Why
Don't know / general purpose / gears and bushings	POM (Delrin)	Machines the best of any plastic. Low moisture uptake. Good strength and stiffness. Covers 60–70% of our plastic work.
Need metal-like strength at high temperature	PEEK	260°C continuous, 90–100 MPa tensile. Replaces aluminum in aerospace and medical. But costs 10–15x more than POM.
Wear pads, bearings, rollers (moderate load)	Nylon (PA6 / PA66)	Good toughness, self-lubricating. Cheaper than PEEK. But absorbs moisture — see below.
Low-friction seals, chemical resistance, food contact	PTFE (Teflon)	Lowest friction of any solid, chemically inert. Extremely difficult to machine — avoid CNC if possible.
Electrical insulation + high temperature (170°C)	PEI (Ultem)	Strong, flame retardant, good electrical properties. Used in aerospace interiors and electronics housings.
Transparent cover, lens, window	Polycarbonate (PC)	Impact resistant, optically clear. Good for prototype enclosures. Machines well.
Wear strips, chute liners, food cutting boards	UHMWPE	Extremely tough, low friction, FDA compliant. Very difficult to hold tight tolerances.
Budget is the driver	POM or Nylon	Both are widely available in standard sizes and priced competitively. POM is safer for tight tolerances.
Medical / food contact / FDA requirement	PTFE, POM-C, or UHMWPE	All have FDA-compliant grades. Verify with your supplier — not all grades of each material are FDA approved.

Default to POM If you're unsure and the application doesn't demand extreme temperature, transparency, or chemical exposure, start with POM. It machines the easiest, holds tolerances best, and rarely causes problems. You can always upgrade to PEEK or PEI later if testing shows it's needed.

Data at a Glance

Plastic	Trade Name	Density (g/cm³)	Tensile (MPa)	Max Temp (continuous)	Machinability	Moisture Absorption	Cost Level	Typical Use
POM-C	Delrin, Celcon	1.41	70	85–100°C	Excellent	Low (0.2%)	Low	Gears, bushings, fittings, valves
PEEK	Victrex, Ketron	1.30	90–100	260°C	Difficult	Low (0.5%)	Very high	Aerospace brackets, medical implants, semiconductor
PA6 / PA66	Nylon	1.14	80	120°C	Good	High (2.5%)	Low	Bearings, wear pads, rollers, pulleys
PTFE	Teflon	2.20	25–35	260°C	Very difficult	None	Medium	Seals, gaskets, chemical linings
PEI	Ultem 1000	1.27	105	170°C	Fair	Low (0.25%)	High	Electrical connectors, aerospace interiors, IC sockets
PC	Lexan, Makrolon	1.20	65–70	130°C	Good	Low (0.2%)	Low	Transparent covers, lenses, prototype enclosures
UHMWPE	Tivar, Polystone	0.93	40	80–100°C	Difficult	Low	Low	Wear strips, chute liners, food cutting boards

Cost reality check POM rod (50mm dia) runs roughly $10–20/kg in China. PEEK rod of the same size is $150–300/kg. That 10–15x material cost difference is real — don't specify PEEK unless the application actually demands it. For most mechanical parts, POM or Nylon handles the job at a fraction of the price.

POM (Delrin / Acetal) — The Workhorse

POM is what we reach for first when a customer says "plastic part." It cuts cleanly, holds tolerances, doesn't absorb much moisture, and costs a fraction of high-performance polymers. If you're new to machining plastics, learn on POM first — everything else is harder.

POM-C vs POM-H — Does It Matter?

Property	POM-C (Copolmer)	POM-H (Homopolymer)
Trade name	Celcon, Hostaform C	Delrin (DuPont)
Tensile strength	60–70 MPa	70–80 MPa
Crystallinity	Lower (more stable)	Higher (slightly stronger)
Acid resistance	Better	Fair (attacked by strong acids)
Dimensional stability	Slightly better	Good
Cost	Similar	Similar (Delrin brand premium ~10%)
Availability	Widely available	Widely available

For CNC machining, the difference is small. POM-H (Delrin) is slightly stronger and has better fatigue resistance, which matters for gears and moving parts. POM-C has better chemical resistance and slightly less thermal expansion. In practice, most shops don't worry about it unless the application is borderline on a specific property.

Machining POM — Sweet Spot Parameters

POM is forgiving. You can get decent results with a wide range of parameters. Here's what works well in our shop:

Operation	Speed (m/min)	Feed	Doc	Notes
Roughing (end mill)	300–500	0.15–0.30 mm/tooth	2–5 mm	2-flute carbide. Aggressive — POM cuts fast.
Finishing (end mill)	500–800	0.08–0.15 mm/tooth	0.2–0.5 mm	Sharp tool, light cut. Polish-quality finish at high speed.
Drilling (φ6–12mm)	50–100	0.10–0.20 mm/rev	—	Peck cycle for deep holes (>3xD). Standard drill point works.
Tapping	20–40	—	—	Use 2-flute spiral flute taps. Thread forming taps work well.
Turning (OD)	200–400	0.10–0.25 mm/rev	1–3 mm	Sharp insert, polished rake face for good finish.

POM thermal expansion POM's coefficient of thermal expansion is roughly 10x that of steel (110 vs 11 μm/m·°C). If you're holding ±0.02mm tolerances, the heat from machining alone can cause 0.05–0.1mm size variation. Use air blast or mist coolant, take light finishing cuts, and let the part cool before final measurement.

Moisture — Not a Big Problem

POM absorbs very little moisture (0.2% at saturation). Dimensional change from moisture is negligible for most applications. You don't need to pre-dry POM before machining unless you're working to very tight tolerances (<0.01mm) in a high-humidity environment. Even then, the effect is small compared to thermal expansion.

PEEK — When It's Worth the Cost

PEEK is the supercar of engineering plastics. It does things no other polymer can: continuous use at 260°C, tensile strength approaching aluminum, chemical resistance to almost everything, and biocompatibility for medical implants. It also costs as much as a supercar relative to other plastics.

When to Actually Use PEEK

Application	Why PEEK, Not Something Else
Aerospace structural brackets	Must survive 200°C+ with specific strength. POM and Nylon can't. Weight savings vs aluminum is 40–50%.
Medical / surgical implants	Biocompatible, sterilizable (autoclave), X-ray transparent. Nothing else checks all three boxes.
Semiconductor wafer handling	Must withstand plasma etching chemicals and high temp. PTFE is too weak structurally.
Oil & gas downhole components	High pressure, high temperature, sour gas exposure. PEEK survives where POM degrades.
Bearings in high-temp environments	POM softens above 85°C. PEEK retains strength to 260°C.

Don't default to PEEK We regularly see drawings specifying PEEK where POM would work fine. The reasoning is usually "we want the best." That's not how material selection works. PEEK costs 10–15x more per kg and machines 3–4x slower. Unless the application demands high temperature, chemical resistance beyond POM's capability, or biocompatibility, you're overpaying. Run the numbers before specifying it.

Machining PEEK — Challenges and Solutions

PEEK is semi-crystalline and abrasive. It dulls tools faster than you'd expect from a "plastic." Here's what you need to know:

Operation	Speed (m/min)	Feed	Doc	Notes
Roughing (end mill)	150–250	0.08–0.15 mm/tooth	1–3 mm	Uncoated carbide OK for short runs. Diamond-coated for production.
Finishing (end mill)	200–350	0.05–0.10 mm/tooth	0.1–0.3 mm	Sharp tool is critical. Dull tool = delamination at the surface.
Drilling	40–80	0.05–0.12 mm/rev	—	Peck cycle mandatory. PEEK chips are stringy and pack the flute.
Turning	150–250	0.08–0.15 mm/rev	0.5–2 mm	Use sharp finishing inserts with polished rake face.

Tool wear is real Uncoated carbide tools last about 30–60 minutes of cutting time on PEEK before noticeable flank wear. Diamond-coated tools last 5–10x longer. If you're machining a batch of 50+ PEEK parts, the diamond tooling pays for itself. For a one-off prototype, uncoated carbide works fine — just check tool wear frequently.

Thermal Management with PEEK

PEEK has low thermal conductivity (0.25 W/mK — roughly 1/700th of aluminum). Heat generated at the cutting edge stays concentrated in a small zone. This causes two problems: localized thermal expansion (affecting dimensional accuracy) and potential thermal degradation of the surface (the material can start to soften or discolor above 340°C).

Solution: Use air blast or minimal mist coolant. Flood coolant is generally not recommended for PEEK because it can cause thermal shock cracking. Air blast clears chips and cools the cutting zone without the shock risk. Keep cutting speeds moderate — don't try to run PEEK at POM speeds.

Pre-drying PEEK

PEEK absorbs some moisture (0.5% at equilibrium). For most machining operations this isn't critical, but for high-temp applications or aerospace parts with tight tolerances, dry the material first: 120–150°C for 3–4 hours in a convection oven. Store in a desiccant bag if not machining immediately after drying.

Nylon (PA6 / PA66) — The Moisture Problem

Nylon is tough, wears well, and costs less than POM. The problem is water. Nylon absorbs moisture like a sponge — up to 2.5% by weight at 50% relative humidity. This causes dimensional swelling (up to 0.3% linear), reduces stiffness by up to 50%, and changes the machining behavior dramatically. If you don't account for moisture, your parts will be the wrong size.

Moisture Effects on Nylon Properties

Condition	Moisture %	Dimensional Change	Tensile Strength	Stiffness
As-received (dry storage)	0.2–0.5%	Near nominal	80 MPa	High (dry and stiff)
Oven-dried	<0.1%	Minimal	80–85 MPa	Highest
Equilibrium at 50% RH	1.5–2.5%	+0.2–0.3% linear	55–65 MPa	30–50% lower
Saturated (immersed)	8–10%	+1.0–1.5% linear	40–50 MPa	60–70% lower

Pre-drying Nylon — Do It Right

For any part with tolerances tighter than ±0.1mm, pre-dry the nylon before machining. The standard procedure:

Step	Detail
Dry temperature	80–100°C for PA6/PA66. Do NOT exceed 120°C — nylon oxidizes and discolors.
Dry time	4–8 hours for rod/bar stock up to 50mm. Larger sections need longer (12–24 hours).
Verify	Weight should stop decreasing. Compare to fully dry weight spec from supplier.
Machine promptly	Nylon reabsorbs moisture quickly. Machine within 4–6 hours of removing from the oven. Keep wrapped in plastic film between operations.
Final dimension	If the part will operate in a humid environment, consider machining slightly undersize to account for equilibrium moisture uptake.

Design around moisture If your nylon part operates in a wet environment (underwater, washdown, outdoor), it WILL grow. Don't fight it — design for it. Either machine the part in the dry state and accept that it'll grow to equilibrium dimensions in service, or pre-condition the material to the expected service humidity before machining. The second approach gives more predictable final dimensions.

Machining Nylon

Operation	Speed (m/min)	Feed	Doc	Notes
Roughing	200–400	0.12–0.25 mm/tooth	2–4 mm	Sharp 2-flute carbide. Nylon cuts fast but melts easily.
Finishing	300–600	0.06–0.12 mm/tooth	0.2–0.5 mm	Light cuts. Melting is the main risk.
Drilling	40–80	0.08–0.15 mm/rev	—	Peck cycle. Nylon re-welds chips if you don't clear them.

Nylon melts, it doesn't cut clean If you see stringy, woolly chips and a gummy surface finish, you're generating too much heat. Reduce speed or increase feed to get proper chip formation. Air blast helps. Nylon has a low melting point (~220°C) and poor thermal conductivity — heat builds up fast.

Nylon 6 vs Nylon 66 vs Cast Nylon (MC)

Property	PA6	PA66	MC Nylon (cast)
Melting point	220°C	260°C	N/A (monomer cast)
Max service temp	80–100°C	120°C	100–120°C
Moisture absorption	Higher (~2.7%)	Moderate (~2.5%)	Lower (~1.5%)
Stiffness	Lower	Higher	Moderate
Availability	Rod, sheet, tube	Rod, sheet, tube	Mostly large tubes and sheets
Best for	General purpose	Higher temp	Large parts, bearings

PTFE (Teflon) — Handle With Care

PTFE has the lowest coefficient of friction of any solid material (0.05–0.10) and resists virtually every chemical. That's the good news. The bad news: it's soft (tensile 25–35 MPa), creeps under any sustained load, deforms under clamping pressure, and is extremely difficult to machine to tight tolerances. If you need CNC precision, PTFE is usually the wrong choice.

The Deformation Problem

PTFE has a cold flow (creep) rate that's 100–1000x higher than POM or PEEK. What this means in practice: if you clamp a PTFE part in a vise, it deforms. Release the vise, and the part doesn't spring back — it stays deformed. Machining it to ±0.05mm is already pushing it. ±0.01mm is unrealistic.

How to Hold PTFE for Machining

Technique	When to Use	Detail
Soft jaws with wide contact	General milling	Use aluminum soft jaws machined to the part profile. Maximum contact area minimizes localized pressure.
Double-sided tape + vacuum	Thin sheets, face milling	Tape the sheet to a flat plate. Works for features on one side only.
Low-pressure workholding	Any critical feature	Use the minimum clamping force that holds the part securely. Test on scrap first.
Filler-reinforced PTFE	When you need better machinability	PTFE filled with glass fiber, carbon, or bronze is significantly stiffer and easier to machine. Trades some chemical resistance and purity.

Machining PTFE

Operation	Speed (m/min)	Feed	Notes
Roughing	150–300	0.10–0.20 mm/tooth	Sharp tools, light cuts. PTFE is gummy — chips stick to the tool.
Finishing	200–400	0.05–0.10 mm/tooth	Zero rake or slightly negative rake helps cut clean instead of pushing.
Drilling	30–60	0.05–0.10 mm/rev	Peck cycle every 1–2mm. PTFE grabs the drill and elongates the hole.

PTFE health warning When PTFE is heated above 350°C (which can happen at the cutting edge with dull tools or excessive speed), it decomposes and releases fumes that can cause polymer fume fever (flu-like symptoms). Use sharp tools, moderate speeds, and good ventilation. This is a real risk, not theoretical.

Consider molded blanks instead of CNC For seals, gaskets, and simple profiles, it's usually cheaper and more accurate to have PTFE compression-molded to near-net shape. CNC machining PTFE is a last resort. Talk to your supplier about molded blanks — you'll get better parts at lower cost.

PEI (Ultem) — High-Temp Electrical Workhorse

PEI (polyetherimide) sits between POM and PEEK in both performance and price. It's amber-colored (naturally translucent), inherently flame retardant (UL94 V-0), and has excellent electrical insulation properties. The main use cases are in aerospace interiors, electrical connector housings, and semiconductor fixtures.

Property	PEI (Ultem 1000)	PEI + 30% Glass	POM (for reference)	PEEK (for reference)
Tensile (MPa)	105	150	70	90–100
Max temp	170°C	180°C	85°C	260°C
Flame rating	UL94 V-0	UL94 V-0	HB (burns)	V-0
Dielectric strength	33 kV/mm	28 kV/mm	20 kV/mm	20 kV/mm
Relative cost	3–5x POM	4–6x POM	1x	10–15x
Machinability	Fair	More abrasive	Excellent	Difficult

PEI is tougher to machine than POM but easier than PEEK. The main issue is that it's more abrasive than it looks — standard carbide tools wear faster than expected. Glass-filled PEI is significantly more abrasive and will eat through tools quickly. Use diamond-coated tooling for glass-filled PEI if you're running more than a few parts.

When to choose PEI over PEEK If your application needs 170°C capability (not 260°C), flame retardancy, or high dielectric strength, PEI does the job at roughly one-third the material cost of PEEK. The aerospace and electronics industries use PEI extensively for exactly this reason.

Surface Treatment for Plastics

Plastics are limited in surface treatment options compared to metals. Here's what actually works and what doesn't, based on our experience.

Treatment	POM	PEEK	Nylon	PTFE	PEI	PC	Notes
As-machined	Good finish	Good finish	Good finish	Fair (creeps)	Good	Good (clear)	Most plastic parts ship as-machined. Polish the tool path for better finish.
Bead blast	Works well	Works well	Works well	Deforms	Works	Frosts surface	Use low pressure (2–3 bar). Fine glass beads (100–200 micron).
Polishing	Mirror possible	Good	Good	Not practical	Fair	Optical polish	Progress through abrasives 400–2000 grit, then polish compound.
Painting	Needs primer	Needs primer	Good adhesion	Nothing sticks	Good	Needs primer	PTFE is famously non-stick — no paint or coating adheres without special surface treatment (sodium etch).
Anodizing / plating	No	No	Electroless only	No	No	No	Plastics don't anodize. Electroless nickel plating on nylon works but is niche.
Laser marking	Good contrast	Good	Good	Melts	Good	Cracks	Low-power fiber laser (10–20W). Test on scrap first.
Dyeing / coloring	Limited	No	Yes	No	No	Limited	Nylon absorbs dye well. This is why nylon is used for colored mechanical parts.

The 80/20 rule Most machined plastic parts don't need any surface treatment. A well-set-up CNC with a sharp tool and the right feeds/speeds produces a surface finish of Ra 0.8–1.6 μm on POM and Nylon, which is good enough for most applications. If the customer wants a specific finish, specify it upfront — post-processing plastics adds cost and lead time.

Machining Plastics — Rules of Thumb

Plastics machine differently from metals. The same intuition that works on aluminum will get you in trouble on nylon. These rules come from years of trial and error.

Speeds and Feeds

Rule	Why
High speed, moderate feed	Plastics cut best at high spindle speeds with moderate feed per tooth. The high speed gives clean shearing; moderate feed prevents heat buildup.
Sharp tools, always	A dull tool generates heat instead of cutting. On plastics, heat = melting = bad surface finish and dimensional error. Replace tools at first sign of wear.
2-flute end mills preferred	More flute clearance means better chip evacuation. Plastics produce larger chips than metals. 3-flute works on POM but 4-flute packs up on Nylon and UHMW.
Zero or slightly positive rake	Positive rake cuts clean. Negative rake pushes the material and generates heat. Exception: PTFE benefits from zero or slightly negative rake to prevent grabbing.
Light depth of cut	Heavy cuts generate too much heat. Rough with 2–4mm DOC, finish with 0.1–0.3mm DOC. Multiple light passes beat one heavy pass on plastics.

Coolant — To Use or Not

Plastic	Coolant recommendation	Why
POM	Air blast preferred, mist OK	POM doesn't absorb coolant. Chips clear well with air. Coolant adds cost and mess without much benefit.
PEEK	Air blast strongly preferred	Flood coolant can cause thermal shock cracking. Air clears chips and cools gradually.
Nylon	Air blast, mist acceptable	Nylon doesn't need coolant. Air is sufficient. If using mist, parts need to be dried before coating.
PTFE	No coolant — air only	PTFE doesn't benefit from coolant. Air blast for chip clearing only.
PEI	Air blast preferred	Similar to PEEK — air blast is sufficient and avoids thermal shock risk.
PC	Air blast, light mist OK	Polycarbonate can crack from thermal shock. Use air blast. Mist is acceptable if needed for deep holes.
UHMWPE	Air blast only	UHMWPE is waxy — coolant makes it slippery and hard to hold.

The general rule: skip flood coolant Unlike metals, most engineering plastics don't benefit from flood coolant. Air blast is usually better for chip removal and temperature control. Flood coolant on plastics creates a mess, adds no significant cooling benefit (because plastics have low thermal conductivity), and can cause problems: nylon absorbs water, PC can crack from thermal shock, and PEEK can develop microcracks. Use air blast as your default.

Tooling Choices

Tool Type	When to Use	Notes
Uncoated carbide	POM, Nylon, PC — most jobs	Sharp edge, good tool life, cost-effective. Default choice for most plastics.
Diamond-coated carbide	PEEK, glass-filled PEI, production runs	5–10x tool life on abrasive plastics. Worth the cost for batches of 20+ parts.
PCD (polycrystalline diamond)	Large PEEK production runs (100+ parts)	Best tool life but expensive. Only justified for high-volume production.
HSS	PTFE, one-off prototypes	Works but dulls fast. Acceptable for soft plastics and short runs.
Sharp-ground drill bits	All plastics	Standard 118° point is fine for POM and PC. Use a sharper point (90° or split point) for PTFE and UHMW to prevent grabbing.

Workholding for Plastics

Plastics are soft — standard metal workholding techniques can damage or deform the part. Key principles:

Rule	Detail
Distribute clamping force	Use soft jaws, custom fixtures, or wide-area clamping. Never use standard vise jaws directly on plastic — they'll leave marks and can crush the part.
Minimize clamping pressure	Use just enough force to hold the part. Test on scrap material first. For thin-wall parts, consider vacuum workholding or double-sided tape.
Machine in stages	Rough all features, release clamping pressure, re-clamp with less force, then finish. This reduces distortion from clamping stress.
Account for springback	When you release clamping force, some plastics (especially PTFE and UHMW) spring back slightly. Machine slightly undersize if tight tolerances are needed.

Procurement Tips

Getting the right plastic stock matters more than most people think. Material quality varies significantly between suppliers, especially in China. Here's what we've learned.

Tip	Detail
Specify the grade, not just the material name	"POM" is not enough. Specify POM-C or POM-H, and the supplier's grade name (e.g., DuPont Delrin 500P, Ticona Celcon M90). Different grades have different fillers, molecular weights, and machining characteristics.
Sheet vs rod — which is cheaper?	For flat parts, sheet is usually cheaper (less machining waste). For cylindrical parts, rod. For complex geometries, rod is often the only option in standard sizes. Budget 30–50% material waste for plastic parts.
Standard sizes in China	POM rod: 6–200mm dia. POM sheet: 5–100mm thick. Nylon rod: 10–300mm dia. PEEK rod: 6–120mm dia. Larger sizes available but with longer lead times (2–4 weeks for PEEK).
PEEK availability	PEEK is not stocked in every city. In Dongguan/Guangzhou area, 3–5 day lead time for common sizes. Special grades (carbon-filled, glass-filled) may need 2–3 weeks. Plan ahead.
Minimum order quantities	POM, Nylon, PC: usually no MOQ — buy by the kilogram. PEEK: some suppliers have a 5–10kg minimum. Sheet material often has a minimum cut charge regardless of weight.
Watch for recycled material	Recycled POM and Nylon are common in China and cost 30–50% less. They machine OK but have inconsistent properties, more voids, and worse surface finish. Use virgin material for precision parts.
Store plastics properly	Keep nylon sealed in plastic bags with desiccant. POM and PC are less sensitive but still benefit from dry storage. PTFE and PEEK are fine in ambient conditions. UV light degrades most plastics over time — store indoors.
Color matters less than you think	Natural (unpigmented) plastics have the most consistent mechanical properties. Black, white, and colored grades have additives that can slightly affect machining behavior. For critical parts, use natural color.

Supplier quality varies enormously We've seen POM rod from different suppliers with the same grade designation that machines completely differently — one cuts clean, the other is gummy and leaves a rough finish. This is usually due to different molecular weight distributions or filler content. Once you find a supplier that produces consistent results, stick with them. Changing suppliers to save 10% on material cost is not worth the setup headaches.

Common Mistakes

We've made most of these ourselves. Learn from our experience.

Mistake	Consequence	Fix
Specifying PEEK when POM suffices	10–15x material cost, 3–4x longer machining time, no performance benefit for the application	Check the actual temperature, chemical, and load requirements. POM handles most mechanical parts at room temperature.
Machining nylon without pre-drying	Part dimensions change 0.2–0.3% as the part absorbs moisture after machining. Tight tolerances are lost within days.	Dry at 80–100°C for 4–8 hours. Machine within 4–6 hours of removal from oven.
Using flood coolant on PEEK or PC	Thermal shock can cause microcracking on PEEK. PC can develop stress cracks. Neither plastic benefits from flood coolant.	Use air blast as the default coolant for all engineering plastics.
Clamping PTFE in a standard vise	Part deforms under jaw pressure. Dimensional accuracy is lost. Surface marks from jaws.	Use soft jaws with wide contact area. Minimum clamping force. Consider molded blanks instead of CNC.
Running dull tools on plastics	Heat generation causes melting, poor surface finish, dimensional errors. POM gets gummy, nylon welds chips back onto the part.	Replace tools at first sign of wear. Plastics are unforgiving of dull cutting edges. When in doubt, put in a fresh tool.
Measuring plastic parts while hot	Thermal expansion gives false readings. A POM part that measures 50.00mm right off the machine may be 49.95mm at room temperature.	Let parts cool to ambient temperature (20–25°C) before final inspection. For tight tolerances, wait 30–60 minutes.
Using 4-flute end mills on nylon or UHMW	Flutes pack with chips, causing poor finish and potential tool breakage. Stringy nylon chips wrap around the tool.	Use 2-flute end mills for better chip clearance. 3-flute is acceptable on POM and PC.
Not accounting for thermal expansion in design	Plastics expand 5–10x more than steel per degree. A 100mm POM part changes 0.1mm with just a 10°C temperature change.	If the operating temperature differs from machining temperature by more than 20°C, calculate the dimensional change and compensate in the design.
Buying recycled POM for precision parts	Inconsistent density, internal voids, poor surface finish. Tolerances are unpredictable.	Use virgin (natural) material for any part with tolerances tighter than ±0.05mm. Recycled is fine for non-critical applications.
Painting PTFE without surface treatment	Paint peels off immediately. Nothing sticks to PTFE without chemical surface modification.	If PTFE must be painted, use sodium naphthalenide etching (specialized process). Better: avoid painting PTFE entirely.

Quick tolerance guide by plastic POM: realistic to ±0.02mm with care. Nylon (dry): ±0.03–0.05mm. PEEK: ±0.02–0.03mm. PEI: ±0.03mm. PC: ±0.03–0.05mm. PTFE: ±0.1mm at best. UHMW: ±0.1–0.2mm. Anything tighter than these ranges is asking for trouble on a consistent basis.

← Copper & Brass

CNC Milling →