Machining Plastics FAQ: Feeds, Speeds, and Techniques

Plastics machine differently from metals in almost every respect—they have lower thermal conductivity, wider coefficient-of-thermal-expansion (CTE) ranges, and widely varying hardness and brittleness. Getting clean dimensions requires matching your speeds, feeds, tool geometry, cooling method, and workholding approach to the specific material. This FAQ answers the most common questions machinists and engineers ask when setting up plastic CNC operations, from entry-level engineering resins to high-performance materials like PEEK and Torlon.

What are the recommended feeds and speeds for machining plastics?

There is no single universal answer because cutting parameters depend on the material, tooling, machine rigidity, and the operation type (milling vs. turning vs. drilling). That said, plastics generally run at higher surface speeds than you might expect for soft materials, because the goal is to shear the material cleanly rather than rub it. Plastic has very low thermal conductivity compared to metal, so heat generated at the cut zone stays local rather than dissipating through the workpiece—this means heat buildup happens faster and can cause melting or glazing of the surface if feeds and speeds are not balanced carefully. Practical starting ranges for common materials:

Acetal (Delrin): 600–1,200 sfm, 0.004–0.008 ipt feed, multiple flutes
UHMW polyethylene: 400–800 sfm, 0.006–0.010 ipt, O-flute or single-flute preferred
Nylon: 500–1,000 sfm, 0.003–0.006 ipt
PEEK: 400–700 sfm, 0.002–0.005 ipt, carbide recommended
Polycarbonate: 400–800 sfm, 0.003–0.006 ipt
PTFE: 300–600 sfm, 0.003–0.005 ipt, very sharp tooling required

Run faster than metal equivalents in sfm but use conservative feed-per-tooth to avoid heat buildup. See the acetal machining guide and PEEK machining guide for material-specific starting points.

Should I use air blast or flood coolant when machining plastic?

Air blast is the first choice for most plastics. It removes chips from the cut zone and provides modest cooling without thermal shock or chemical interaction with the workpiece. Flood coolant with water-soluble cutting fluids is acceptable for materials like acetal, nylon, and PEEK but can cause problems in others:

Polycarbonate is susceptible to stress cracking from many cutting fluids—use air or dry cutting only, or confirm coolant compatibility before use.
Nylon absorbs moisture and can swell slightly with prolonged flood coolant exposure, affecting dimensional stability of tight-tolerance parts.
PTFE and UHMW need no coolant and are better served by air blast.

Never use petroleum-based neat oils on amorphous materials without chemical compatibility verification. When in doubt, run dry with air blast and optimize feeds/speeds to minimize heat generation.

What tool geometry works best for plastics?

Sharp tools with high positive rake angles cut plastics cleanly rather than rubbing and generating heat. Key geometry guidelines:

Rake angle: 10–20° positive (higher for soft materials like UHMW and PTFE, lower for harder materials like PEEK or filled grades)
Relief angle: 10–15° to reduce rubbing behind the cutting edge
Helix angle: High-helix (45°–60°) end mills pull chips upward and clear them away from the workpiece
Edge prep: Razor-sharp, no honing or edge rounding—plastics need a clean shearing action
Flute count: Single-flute or two-flute for gummy materials (UHMW, PTFE, LDPE); two-to-four flutes for harder engineering resins

Carbide outperforms HSS on abrasive filled grades (glass-filled nylon, PEEK GF30, Torlon). For unfilled resins, sharp HSS is adequate. See the UHMW machining guide for geometry specific to ultra-high-molecular-weight polyethylene.

Which plastics are most prone to cracking or chipping during machining?

Brittle amorphous thermoplastics are highest risk:

Acrylic (PMMA): Highly notch-sensitive; sharp internal corners, aggressive feeds, and dull tools all cause cracking. Slow down and use coolant-free operation with high positive rake.
Polycarbonate: Cracks from both mechanical stress and solvent attack. Keep tools sharp; avoid flood coolants.
G10 and FR4 and phenolic laminates: Brittle but for a different reason—glass fiber content makes them abrasive and prone to delamination at exit holes. Use carbide, slow feeds, and backing material on breakthrough cuts.
PVDF (Kynar): Can crack if clamped too aggressively or if tools push rather than cut.
Ultem (PEI): Notch-sensitive; avoid sharp internal radii.

Acrylic and polycarbonate should always be annealed before machining tight-tolerance parts. Peck-drilling with chip clearance is especially important in brittle materials.

Should plastics be annealed before or after machining?

Before machining: Annealing relieves residual stress built into the stock during extrusion or casting. This matters most for acrylic, polycarbonate, and Ultem—materials that develop high residual stress during manufacturing. Pre-machining anneal dramatically reduces the risk of cracking during cutting. Typical protocol: 4–8 hours at 10–15°F below the HDT, slow ramp up and down (~25°F/hr).

After machining: A post-machining anneal relieves stress introduced by the cutting process itself and can rescue dimensions if the part warped slightly during machining. Recommended for tight-tolerance parts in any amorphous resin. Anneal time: 2–4 hours at the same temperature range, then slow cool.

Do both when surface finish and dimensional accuracy are critical. The acrylic machining guide covers annealing schedules in detail for that material.

What dimensional tolerances are realistically achievable when machining plastics?

General achievable tolerance ranges by category:

Material class	Routine	With care
Semi-crystalline (acetal, nylon, PEEK)	±0.003–0.005 in	±0.001–0.002 in
Amorphous (PC, acrylic, Ultem)	±0.003–0.005 in	±0.002–0.003 in
PTFE / UHMW (soft, high CTE)	±0.005–0.010 in	±0.003–0.005 in
Filled composites (G10, phenolic)	±0.003–0.005 in	±0.002–0.003 in

The limiting factor is usually thermal expansion, not machine accuracy. Plastics expand 5–15× more per degree than steel. For features tighter than ±0.002 inches, control part temperature during machining, allow thermal equalization before final passes, and check dimensions after the part has stabilized at room temperature. Review material-specific specifications on the acetal specifications page

How do I achieve a smooth surface finish when machining plastics?

Surface finish on plastics is heavily influenced by tool sharpness, chip clearance, and feed rate:

Sharp tools: A dull tool smears rather than cuts, leaving a cloudy or torn surface. Replace or resharpen more frequently than you would for metal.
High spindle speed / light finish pass: Take a 0.005–0.010-inch finish pass at high speed and low feed to shear rather than plow the surface.
Chip evacuation: Chips re-cut into the surface cause scratches. Air blast continuously during finishing passes.
Climb milling: Typically produces better finishes in plastics than conventional milling because the chip thickness starts thick and thins—less rubbing at exit.
Polishing: Acrylic can be flame-polished or buffed to optical clarity. Most other plastics can be wet-sanded with 400–800 grit and buffed.

For optically clear parts, see the polycarbonate machining guide and acrylic material hub for polishing techniques.

How do I stress-relieve plastic parts after machining?

Stress relief is essentially the same process as post-machining annealing: controlled heating to slightly below the material's HDT, holding for 2–4 hours (longer for thick sections), followed by slow cooling at 25°F per hour or less. Key material temperatures:

Acetal: 220°F (104°C) for 2–4 hours
Polycarbonate: 250°F (121°C) for 2–4 hours
Acrylic: 165–180°F (74–82°C) for 4–8 hours (lower than most—acrylic's HDT is modest)
PEEK: 300–350°F (149–177°C) for 2–4 hours
Nylon: 200–250°F (93–121°C), dry-heat oven only
Ultem (PEI): 340–360°F (171–182°C) for 2–4 hours
Acrylic: Part size matters—soak time for parts over 1 inch thick should be extended to 6–8 hours to ensure the core reaches temperature

Use a circulating air oven, not a static oven, for uniform temperature distribution. Do not exceed the material's HDT—even briefly—or you will introduce permanent deformation. Parts should be supported evenly on a flat fixture during annealing so they cannot sag; use aluminum cradles or level support plates for precision parts. Parts with large unsupported spans can bow significantly at temperature if not properly fixtured. Rapid cooling after the anneal—such as removing parts directly from a hot oven into room-temperature air—reintroduces residual stress, defeating the purpose. Always let the oven cool with the door closed or on a slow ramp. See the PEEK machining guide for high-temperature anneal protocols.

How do I hold plastic parts securely in a CNC fixture without distorting them?

Over-clamping is a major cause of dimensional problems and cracking in plastics. Plastics compress and deform under clamp load far more than metals. Best practices:

Soft jaws: Machine jaws from aluminum or even plastic to match the part geometry—spreads clamping force over more area.
Vacuum fixtures: Excellent for flat sheet parts. Distributes hold-down force evenly without inducing bending stress.
Double-sided tape and adhesive: For thin sheet work, double-sided tape on a flat plate eliminates clamp marks entirely.
Low-clamp-force vises: Use a torque wrench or spring-loaded vises to limit clamping force.
Tabs and bridges: Leave tabs to hold the part in the stock, then trim—avoids vibration on the last pass.

For soft materials like UHMW and PTFE, even light clamping can deform the part; vacuum fixturing is strongly preferred.

When should I use a single-flute end mill versus a multi-flute end mill for plastics?

Single-flute end mills maximize chip pocket size, which is the primary concern with gummy, soft, or tacky materials. When chip evacuation is poor, material welds back into the cut zone, causing pulled surfaces and tool breakage. Use single-flute for:

UHMW polyethylene, LDPE, polypropylene, PTFE (all tend to gum)
Any deep-slot operation in soft thermoplastics
Small-diameter cuts where chip load per tooth needs to be highest

Multi-flute (3–4 flute) tools are appropriate for harder, more dimensionally stable materials:

Acetal (Delrin), nylon, PEEK, Ultem, phenolic laminates
Light finishing passes in any engineering resin
Operations where surface finish matters more than chip clearance

Two-flute end mills are a good compromise for most engineering-grade thermoplastics. Avoid 4+ flute tools in soft plastics—they will pack with chips. See the nylon material hub for more on machining semi-crystalline polyamides.

Can I drill plastic with standard metal-working drill bits?

Standard twist drills work on most plastics but often produce poor results—tear-out at exit, melting, and out-of-round holes. For better results:

Regrind to a 90–118° point angle (flatter than standard) and increase the relief angle to reduce friction
Slow feed, fast speed: Let the drill shear rather than push through
Peck drill: Especially important in deep holes (>2× diameter) to clear chips and prevent heat buildup
Dedicated plastic drill bits: Available with a modified geometry (often called "brad point" for thermoplastics); produce much cleaner holes
Backing material: Clamp a sacrificial plate under the exit side to prevent blow-out in brittle materials like acrylic, G10, or phenolic

For threaded holes, tap sizes for plastics typically need slightly more clearance than metal—consult the specific material's machining guide, such as the acetal machining guide

PTFE (Teflon) and UHMW polyethylene are the most challenging because of their extreme softness and tendency to deform rather than cut—they require very sharp tools, high speeds, light cuts, and careful fixturing. On the opposite extreme, G10 and FR4 and phenolic laminates are difficult because of abrasiveness: the glass fibers dull carbide rapidly, require diamond-coated or PCD tooling for production runs, and generate fine abrasive dust that requires respiratory protection. High-performance resins like PEEK and PAI (Torlon) machine well but are unforgiving of dull tools or heat. Polyimide (Vespel) is arguably the most demanding: extreme hardness, brittle, and requires specialized tooling and very slow feeds.

More related guides

Useful jumps for further reading:

Material hubs

Industries