Skip to content
M
MakerStage

Acetal Behaves More Like Soft Aluminum Than Like Other Plastics.

Engineers who have struggled with nylon's stringy chips or polycarbonate's thermal sensitivity are often surprised by how cleanly acetal machines. POM produces short, predictable chips at high speeds, holds tight tolerances without humidity conditioning, and requires no coolant. The key variables to control are tool sharpness and depth of cut on thin walls. Get those right and acetal is a pleasure to machine.

Section 1 of 6

Why Acetal Machines So Well

Understanding the material behavior helps you set up cuts correctly from the start, not after the first scrap part.

Semi-Crystalline Structure

POM's high crystallinity (75–85%) makes it behave like a hard, brittle solid at the cutting edge — chips fracture cleanly rather than tearing. This is why acetal chips are short and predictable, unlike amorphous plastics (PC, ABS) that tend to smear.

Low Thermal Sensitivity

POM has higher thermal conductivity (0.31 W/m·K) than most plastics and a relatively high melting point (175°C POM-H). The cutting zone stays below the thermal degradation point at normal plastic machining speeds. Compare to PTFE or polyethylene that melt and smear at modest speeds.

Dimensional Stability

Moisture absorption below 0.25% in 24 hours means the part dimensions do not change significantly between machining and inspection. With nylon, you must condition stock to equilibrium moisture content before machining to avoid tight dimensions "relaxing" after cutting. Acetal needs no conditioning.

Section 2 of 6

Speeds and Feeds Reference

If you're setting up your first acetal job, start with these parameters — they work for unfilled POM on any standard CNC lathe or mill with carbide tooling. All values for unfilled acetal POM with standard uncoated carbide tooling. Filled grades (PTFE, glass) use the same parameters; carbon-filled grades may require slightly lower speeds due to increased tool wear from carbon fiber reinforcement.

OperationCutting SpeedFeed RateDepth of CutNotes
OD Turning (roughing)300–500 SFM (90–150 m/min)0.006–0.010 in/rev (0.15–0.25 mm/rev)0.050–0.150 in (1.3–3.8 mm)Carbide insert, positive rake, sharp edge
OD Turning (finishing)400–600 SFM (120–180 m/min)0.002–0.005 in/rev (0.05–0.13 mm/rev)0.005–0.020 in (0.13–0.51 mm)Sharp insert mandatory — dull insert smears POM
Boring (ID turning)300–500 SFM (90–150 m/min)0.003–0.007 in/rev (0.08–0.18 mm/rev)0.030–0.100 in (0.8–2.5 mm)Compressed air for chip clearing in deep bores
Face milling5,000–8,000 RPM (1 in cutter)0.005–0.008 in/tooth (0.13–0.20 mm/tooth)0.020–0.060 in (0.5–1.5 mm)Positive rake face mill; climb milling preferred
End milling (slot/pocket)6,000–10,000 RPM (1/2 in EM)80–150 in/min (2,000–3,800 mm/min)Axial: 0.5–1.0× dia; Radial: 0.3–0.5× dia2-flute high-helix; reduce radial DOC for deep walls
End milling (finishing pass)8,000–12,000 RPM (1/2 in EM)100–200 in/min (2,500–5,100 mm/min)Axial: 0.5× dia; Radial: 0.005–0.020 inLight spring pass improves surface finish to Ra 32–63 µin (0.8–1.6 µm)
Drilling3,000–5,000 RPM (1/4 in drill)0.004–0.008 in/rev (0.10–0.20 mm/rev)Full diameterStandard HSS or carbide; frequent peck cycles on deep holes
Tapping200–400 RPMGoverned by pitchThrough or blindStandard taps; no oversized pilot holes needed (unlike nylon)
Reaming500–1,000 RPM0.005–0.012 in/rev (0.13–0.30 mm/rev)0.005–0.015 in (0.13–0.38 mm) stock removalAchieves H7 bore tolerances; use carbide or HSS spiral-flute reamer

Start Fast, Then Optimize

Acetal is forgiving of aggressive initial parameters. Start at the high end of the speed range and observe chip character: clean, short chips (2–8 mm) indicate optimal cutting; long, stringy chips mean the tool is rubbing; powdery, hot chips mean the material is melting rather than cutting. Adjust from there. Unlike steel, over-speed in acetal typically causes surface melt rather than catastrophic tool failure.

Section 3 of 6

Tool Selection and Geometry

Your tool geometry matters more than your machine when cutting acetal — the wrong cutter will melt and smear POM regardless of your speeds and feeds. Tool geometry matters more than material in plastic machining. The key principle: sharp, positive-rake geometry that cuts cleanly rather than pushing the material.

Turning Inserts

  • Grade: Uncoated carbide (K10–K20); TiN-coated acceptable but not required
  • Geometry: Positive rake angle (10–15°); polished chipbreaker face
  • Nose radius: 0.016–0.031 in (0.4–0.8 mm) for finish passes; larger for roughing
  • Edge prep: Ground and honed, never chipped — POM telegraphs tool wear immediately
  • Tool life: Very long vs steel applications — change when surface quality degrades

End Mills

  • Flutes: 2-flute preferred for slots and pockets; 3-flute acceptable for small depths
  • Helix: 35–45° high-helix for chip evacuation out of the cut
  • Grade: Uncoated carbide (C2/K10); TiAlN or DLC coatings acceptable
  • Diameter: 1/4 in to 1/2 in most common; smaller for fine features
  • Avoid: 4+ flute end mills in deep pockets — chip re-cutting damages acetal surface

Drills

  • Standard HSS twist drills work well for diameters under 1/4 in
  • For precision bores, drill undersize then ream to final dimension
  • Step drills useful for non-standard diameters in sheet material
  • Peck drill cycles for holes deeper than 3× diameter to prevent chip packing
  • Acetal tends to grab at drill breakthrough — maintain feed rate through exit

Taps and Thread Mills

  • Standard HSS or carbide taps in all common thread sizes
  • No oversized pilot holes — acetal does not swell like nylon
  • Spiral-flute taps (gun taps) for through holes; spiral-point for blind holes
  • Thread milling preferred for tight-tolerance threads in precision work
  • Avoid excessive tap speed — heat causes galling at thread root
Section 4 of 6

Tapped Holes vs. Thread Inserts

If your acetal part requires threaded fasteners, the thread size and number of assembly cycles determine whether you tap directly into POM or install brass inserts. Acetal threads are good — but they have limits. Knowing when to tap and when to insert is critical for parts that will be fastened and re-fastened in service.

Thread SizeRecommended ApproachTorque Limit (approx.)Notes
#4-40, #6-32, #8-32Tapped hole2–5 in·lbLight duty — do not overtorque; stripped thread non-recoverable
1/4-20 UNCTapped hole (light duty) or brass insert8–15 in·lb tapped; 30–50 in·lb with insertIf repeatedly assembled/disassembled, use brass press-fit insert
5/16-18, 3/8-16Heat-set or ultrasonic brass insert—Tapped thread marginal at these sizes under structural load; insert preferred
M2, M3, M4Tapped hole (light duty)0.2–1.0 N·mAcceptable for non-structural, non-repeated assembly
M5, M6Brass heat-set insert recommended—Tapped M6 in POM will strip at low torque — use insert for any structural fastening
M8, M10, M12Brass heat-set insert required—Always use inserts for M8 and above; tapped threads too weak for fastener torque spec

Free DFM Review on Every Acetal Order

MakerStage reviews every acetal RFQ for machinability risks before quoting — including thread sizing, thin wall flags, and tolerance callouts that require special tooling. Upload your CAD file and get a quote with DFM feedback included at no charge.

Get a CNC Acetal Quote with Free DFM Review
Section 5 of 6

Common Defects and How to Prevent Them

Most acetal machining defects have one root cause: heat. Learn to read chip character as your primary process indicator.

High severity

Melted or smeared surface finish

Cause: Dull tool generating heat through rubbing rather than cutting; excessively high feed on finishing pass with dull insert

Fix: Replace tool — this defect cannot be fixed with parameter changes on a dull cutter. Sharp insert + reduced surface speed on finishing pass.

Moderate

Chatter marks on OD surface

Cause: Part deflection in chuck (thin walls, long unsupported overhangs); excessive DOC on finishing pass

Fix: Use collet instead of 3-jaw chuck; reduce overhang; take lighter finishing passes; ensure steady rest support for long parts

Moderate

Chips packing in deep bores or blind holes

Cause: POM chips do not evacuate under gravity alone; no coolant to flush

Fix: Use peck drill cycles with full retract; add compressed air blast directed into bore; increase peck depth cycle frequency

Moderate

Oversized bore after reaming

Cause: Reamer deflection in thin-wall section; incorrect reamer allowance (acetal springs back less than metals)

Fix: Leave 0.005–0.010 in for reaming (less than metal practice); support thin walls with plug or fixture during reaming

High severity

Stripped tapped threads

Cause: Overtorquing fastener beyond POM bearing strength; thread too short (< 2× pitch diameter engagement)

Fix: Use brass heat-set insert for M5/1/4-20 and above; ensure minimum 2× major diameter thread engagement

High severity

Centerline voids in bored ID (POM-H stock)

Cause: Pre-existing centerline porosity from rod manufacturing; typically >25 mm diameter stock

Fix: Specify POM-C copolymer for thick-section parts; inspect POM-H stock with sacrificial face cut before full production

Section 6 of 6

DFM Checklist for Acetal Parts

Check these items before sending your CAD file for quoting. Each prevents a costly surprise.

Material Specification

  • Drawing specifies POM-H or POM-C explicitly — not just "acetal"
  • Stock thickness < 25 mm if POM-H specified; POM-C for thicker stock
  • Color specified — natural (white) for FDA applications; black for others
  • FDA-compliant grade called out if food or medical contact

Wall Thickness

  • Minimum wall thickness ≥ 0.060 in (1.5 mm) for machined features
  • Walls < 0.060 in: fixturing plan reviewed with machine shop before order
  • Thin ribs: height-to-thickness ratio ≤ 5:1 without dedicated support fixture
  • Thin-wall bores: fixture plan for reaming to tolerance without distortion

Threads and Fasteners

  • Tapped holes ≤ #10-32 / M5: acceptable for light duty only
  • Threads ≥ 1/4-20 / M6 under structural load: brass insert called out on drawing
  • Minimum thread engagement: 2× major diameter in acetal
  • Fastener torque on drawing does not exceed POM bearing strength

Tolerances and Fits

  • OD tolerances: ±0.002 in standard; ±0.001 in achievable, flag as precision
  • Bore tolerances: ±0.001–0.002 in; H7 bore achievable with reaming
  • No tolerances tighter than ±0.001 in without discussion of fixturing method
  • Running fits: H7/f6 or H7/g6 standard for shafts through POM bushings

Feature Geometry

  • Internal radii ≥ 10% of cavity depth for clean end mill passes
  • Blind holes: specify flat bottom or radius at bottom, not assumed flat
  • Undercuts and T-slots: noted explicitly; require live tooling or secondary setup
  • Chamfers on all external sharp edges: prevents chipping in assembly and use

Surface Finish

  • Default finish Ra 63–125 µin (1.6–3.2 µm, machine finish) is appropriate for most applications
  • Ra 32 µin (0.8 µm) achievable with finishing pass — call out only where functionally needed
  • Bearing surfaces and sliding fits: call out Ra 32–63 µin (0.8–1.6 µm) explicitly
  • No plating or painting on acetal — coatings do not adhere to POM

Further Reading

Common Questions

Frequently Asked Questions

What speeds and feeds for CNC machining acetal?
For turning: surface speed 300–600 SFM (90–180 m/min) with carbide insert; feed 0.003–0.010 in/rev (0.08–0.25 mm/rev). For milling with 1/2 in (12.7 mm) 2-flute carbide end mill: 6,000–10,000 RPM, feed 80–150 in/min (2,000–3,800 mm/min), axial DOC 0.25–0.5× diameter. Sharp tools are critical — dull tools generate heat and smear the surface. No coolant required for most operations; compressed air for chip clearing on deep features.
What tolerances are achievable when CNC machining acetal?
Turned OD tolerances of ±0.001 in (±0.025 mm) are routine on good lathe setups. Bored IDs achieve ±0.001–0.002 in. Flatness and parallelism hold to 0.001–0.002 in/in. POM is dimensionally stable — unlike nylon, it does not change significantly with humidity. The primary challenge is workpiece compliance on thin-wall features, not material instability.
Does acetal need coolant when machining?
Most acetal machining operations require no coolant. POM generates relatively low cutting heat at standard plastic speeds, and flood coolant can cause dimensional changes due to thermal shock and absorption. Compressed air for chip evacuation is preferred — particularly on deep bores and blind pockets. If coolant is used, water-soluble coolant at low concentration is acceptable; avoid oil-based coolant that leaves residue on food-contact parts.
Can you tap threads in acetal?
Yes. Acetal taps very well and produces clean, accurate threads. Use standard tap drill sizes — acetal does not swell into threads like nylon. For production applications requiring thread strength, use brass or stainless heat-set inserts for threads larger than 1/4-20 UNC subject to torque loading. Tapped threads in POM are suitable for light to moderate fastener torque (inspect pilot hole for thread stripping when torquing to spec).
What end mill geometry for acetal?
Two-flute, high-helix (35–45°) end mills in uncoated carbide are the standard choice for acetal. The two-flute geometry provides good chip evacuation in the wide-open flute space; more flutes risk chip packing in plastic at high feed rates. Keep tools sharp — once an end mill is worn to the point of generating heat on steel, discard it before using on acetal. Dull tools create smeared or melted edges on POM that must be re-cut.
How do you hold thin-wall acetal parts for machining?
Thin-wall acetal parts (walls under 0.060 in / 1.5 mm) require careful soft-jaw fixturing. Standard three-jaw chucking distorts thin-wall tubes and rings — use split collets, mandrels, or custom soft jaws that distribute clamping load over the full part circumference. For milled thin plates, double-sided tape or vacuum fixture prevents deflection during light finishing passes. Avoid excessive clamping pressure — acetal is stiff but creeps under sustained compressive load.

Related Resources

Acetal CNC Tolerances
What's achievable — tolerance reference tables
Acetal / POM Guide
Complete material guide with all properties
DFM Best Practices
Design for manufacturability — metals and plastics

Ready to Machine Your Acetal Part?

CNC machining in Delrin (POM-H), acetal copolymer (POM-C), and filled grades. Free DFM review — we catch tolerance and thread issues before your parts are cut.

Get a Free Acetal Quote