Machining Nylon: Speeds, Feeds, Tools & Tips

Nylon machines cleanly when you apply sharp, positive-rake tooling, adequate chip clearance, and controlled heat. The biggest mistakes machinists make with nylon — using dull tooling, flooding with coolant, and ignoring thermal expansion — create dimensions that drift, surfaces that melt, and chips that jam in the cut. This guide covers turning, milling, drilling, and sawing parameters for cast Nylon 6 and extruded Nylon 6/6, with notes on filled grades.

TL;DR

• Use sharp, positive-rake carbide or HSS tools — dull tools generate heat that melts the surface and pushes dimensions
• Nylon chips are long and stringy; use chip breakers, compressed air, or frequent tool retraction to clear
• Avoid flood coolant — it introduces moisture that changes dimensions; use compressed air instead
• Thermal expansion is significant (CTE ~5 × 10⁻⁵ in/in/°F) — rough first, let the part cool, then finish
• Cast nylon 6 machines with less stress release than extruded; for thin-wall or high-precision parts, cast stock is more predictable
• Glass-filled nylon requires carbide tooling and is abrasive to cutters — expect shorter tool life

Why Nylon Machining Requires Different Thinking

Nylon is not metal. Four characteristics require specific technique adjustments:

1. Low thermal conductivity (0.14–0.17 W/m·K vs. ~200 for aluminum): heat concentrates at the cutting zone. A dull cutter generates enough heat to melt the surface, producing smeared finishes and dimensional errors.

2. High coefficient of thermal expansion (CTE ~5 × 10⁻⁵ in/in/°F, roughly 5× steel): a nylon rod heated from 70°F to 140°F during cutting expands ~0.007" per inch of diameter — enough to render mid-cut measurements meaningless.

3. Moisture absorption (2–9%): stock from a bag is near-dry. A part machined dry can become tight in service if it absorbs moisture to equilibrium. Design clearances for the expected service moisture state.

4. Stringy chips: nylon produces long continuous spirals that wrap around tooling, drag across the finished surface, and generate heat marks. Chip management is not optional.

Turning

Tooling Geometry

Use carbide insert tooling or sharp, reground HSS tools with these geometry parameters:

Cutting Speeds and Feeds — Turning

Roughing vs. Finishing:

• Roughing passes: use maximum feed and depth to remove stock quickly; dimensional accuracy is secondary
• Semi-finishing: reduce depth to 0.040"–0.060", stop, wait 10–15 minutes for part to return to ambient temperature
• Finishing pass: 0.005"–0.015" depth, high surface speed, light feed — the part must be at ambient temperature for the dimension to mean anything

Chip Control on the Lathe

Nylon's stringy chips are the main process issue in turning. Strategies:

1. Chip breaker geometry: use an insert with an aggressive chip-breaker groove or grind a breaker notch into HSS tooling
2. Air blast: direct compressed air at the cutting zone from a nozzle — chips clear and temperature stays controlled
3. Retract and clear: on manual lathes, stop and break chips every 5–10 seconds on deep roughing cuts
4. Do not use a long-stringy chip vacuum alone: vacuum will pull the chip into the chip breaker zone and can pull the workpiece if the chip wraps and jams

Milling

Tooling

• End mills: 2-flute or 3-flute HSS or carbide end mills. Fewer flutes = larger chip gullet = better chip evacuation. 4-flute end mills clog quickly on nylon.
• Helix angle: 30°–45° helix for best chip lift out of the cut
• Coating: uncoated carbide or TiN-coated. TiAlN (designed for high-temp metals) is unnecessary and adds cost.

Milling Parameters

Step-over for face milling: 60–75% of cutter diameter. Overlapping passes create better surface finish on nylon than wide, shallow step-overs.

Climb vs. Conventional Milling

Climb milling (conventional CNC practice) is preferred on nylon. Conventional milling tends to lift and pull nylon workpieces against the clamp, and the chip rubbing back through the cut generates heat. Climb milling takes the chip out of the cut immediately.

Drilling and Boring

Drill Selection

Standard jobber twist drills work on nylon but require geometry adjustments:

• Point angle: 90°–118° included angle (standard 118° works; 90° gives a flatter bottom and less grabbing tendency)
• Helix angle: standard (20°–30°); slow-helix drills trap chips — avoid
• Cutting speed: 200–400 SFM for drills (lower than turning, due to chip packing in the flutes)
• Feed: moderate to high — light feeds cause rubbing and heat; 0.004"–0.010" per revolution depending on diameter

Common problem — drill grab: Large drills tend to grab and "screw in" to nylon as they break through the back side. Solutions:

• Reduce feed rate at the breakthrough
• Clamp a backup plate behind the workpiece
• Use a split-point drill (reduces thrust and grab tendency)
• Pilot drill first, then enlarge

Boring for Bearing Fits

For bushing ID bores requiring ±0.001" or better:

1. Drill undersize (leave 0.020"–0.060" per side)
2. Rough bore at 0.010"–0.020" per side
3. Allow full temperature recovery (minimum 15 minutes)
4. Finish bore to dimension in one light pass (0.003"–0.005" per side)
5. Measure only after the part returns to ambient temperature

Sawing

Band saw: Hook-tooth blade, 4–6 TPI for thick plate or 8–14 TPI for thin sheet; 3,000–5,000 SFPM. Feed at a steady rate — slow feeding melts the kerf.

Cold saw / circular saw: Carbide-tipped blade rated for plastics. Maintain a steady feed through the full cut — stopping mid-cut creates a heat ring that can fuse the kerf.

Table saw: Fine-tooth ATB blade (60–80 tooth, 10" blade). Hold sheet firmly to prevent flutter at blade entry.

Dimensional Control and Moisture Management

Sequence for Tight-Tolerance Nylon Parts

1. Condition the stock: open the bag and allow the stock to equilibrate to shop humidity for 24–48 hours before starting (or machine in the as-received dry state and note the difference)
2. Rough machine: remove bulk stock, leaving 0.020"–0.060" per surface
3. Rest the part: allow 1–4 hours minimum (overnight preferred for parts thicker than 1") for heat and stress to relax
4. Finish machine: final cuts at light depth and high surface speed
5. Measure cold: take measurements only after 15–30 minutes at room temperature

Fixturing

Nylon's low rigidity compared to metal means fixturing strategy matters:

• Soft jaws: use aluminum or nylon soft jaws in a 3-jaw chuck; steel jaws can indent nylon under clamping pressure, distorting the bore
• Minimum clamping force: use only enough force to prevent slipping — over-clamping deforms the workpiece
• Long bars (bar feed): support nylon rod with a steady rest or outboard support for bars longer than 4× diameter to prevent whip and chatter
• Vacuum fixtures: effective for flat sheet milling — nylon's smooth underside holds well to vacuum tables; surface must be dry and flat

Special Notes for Filled Grades

Nylatron GS (MoS₂): Machines similarly to unfilled nylon. MoS₂ particles are sub-micron and do not significantly affect tool wear. Use the same parameters as unfilled Nylon 6.

Nyloil (oil-filled): The oil in the matrix can cause slight surface slipperiness — chips do not cling to the workpiece and clearing is actually easier. No special tool geometry required.

Glass-filled (GF33): Glass fiber is abrasive to tooling. Use carbide only — HSS wears rapidly. Reduce surface speed by 40–50% vs. unfilled. Expect tool life 50–75% shorter than with unfilled grades. Burrs on edges are sharper and harder to break; plan for deburring with a file or fine abrasive.

For grade-specific properties that affect machining behavior, see the nylon grades guide. For stock sizes and what's available to machine from, see the nylon specifications page.

Related Guides

More related guides

Cross-cluster suggestions to help shoppers and engineers explore adjacent topics:

Applications

• Bushings Bearings
• Wear Strips Guide Rails
• Gears

Industries

• Food Beverage
• Automotive

Compare to other materials

• Acetal Vs. Nylon
• Nylon Vs. Uhmw
• Nylon Vs. Cotton Phenolic

Frequently asked questions — Nylon FAQ