Guides / Machining

What Tolerances Are Realistic on a Machined PEEK Part

September 20, 2026

Sources: manufacturer datasheets and published standards. See editorial standards.

A PEEK drawing with metal tolerances on every feature gets one of two answers: a quote far higher than the part deserves, or parts that measure fine at the shop and wrong at your bench. Neither is the shop being difficult. PEEK simply moves more than metal, and it moves for reasons you can plan around.

Start from these numbers

What	Realistic on PEEK
General machined features	±0.05 mm
Small annealed features, carbon filled stock	±0.025 mm
Very short features, temperature controlled shop	a little under ±0.025 mm
Bore roundness on a thin walled part	±0.03 mm after stress relief
Flatness on a thin plate part	0.1 mm over 100 mm is a fair starting point
Surface finish, finishing pass	Ra 0.8 µm
Surface finish, polished tool and light passes	Ra 0.4 µm

These are the values shops quote without a long conversation. Anything tighter is possible on some features and impossible on others, and the difference is geometry, not skill.

Why the material fights you

Thermal expansion. Unfilled PEEK expands about 47 µm/m·K below the glass transition at 143 °C. Steel is around 12. A 100 mm feature that is on size at 20 °C grows about 0.06 mm by the time the part reaches 33 °C. A warm shop and a cold inspection room are enough to argue about a ±0.025 mm callout.

Internal stress. Extruded stock holds stress from cooling. Machining releases it unevenly and the part relaxes into a new shape over the following hours. This is why annealing between roughing and finishing exists, and why a part that passed inspection can fail a week later.

Low thermal conductivity. Heat from the cut stays near the cut. A part can grow while it is being machined, which is why shops take light finishing passes with plenty of air or coolant rather than one heavy pass.

Clamping. PEEK has a modulus around 3.5 to 4 GPa unfilled, roughly one fiftieth of steel. Clamp a thin walled part hard and you machine it round while it is squeezed oval. Soft jaws, light pressure and support under thin sections are part of the process.

Tolerance at a temperature, not in the abstract

This is the single most useful change you can make to a PEEK drawing. If a fit has to work at 180 °C, write that on the drawing next to the tolerance. Then everyone knows what has to be true and where.

Three ways this plays out:

• Cold fit, hot service. The shop machines a clearance that closes as the part warms. You need the service temperature to calculate it.
• Hot fit, hot inspection. Rare, expensive and sometimes the only honest answer for a sealing face.
• Filled grade instead. Carbon filled PEEK expands about half as much as unfilled, which is why it ends up in fixtures and wafer handling parts. See CF30 vs GF30 for the trade.

What to tolerance, and what to leave alone

Every tight callout adds a finishing pass, an inspection step and scrap risk on an expensive block. A useful pass over the drawing:

1. Mark the features that actually fit something. Bores, shoulders, seal faces, slot widths that hold a blade.
2. Put general tolerance on everything else. ±0.1 mm is fine for outside profiles that touch nothing.
3. Remove symmetry and parallelism callouts you copied from a metal part. They often force a fourth setup.
4. Add a radius to internal corners. A sharp corner is a stress concentration and a place where a cutter has to slow down.
5. Say where the datum is and pick one the shop can actually clamp on.
6. State the inspection temperature if a fit is under ±0.05 mm.

Measuring a plastic part

Two habits cause most tolerance arguments:

Measuring too soon. A part fresh off the machine is warm and has just been released from the vice. Let it sit, then measure.

Measuring with too much force. A micrometer with a ratchet stop reads a PEEK part smaller than a light touch does, because the material yields. For anything under ±0.05 mm, non-contact measurement or a fixed force gauge is the honest way.

If the part is critical, agree the method before the first batch. Shops are used to this conversation and it costs nothing.

When the tolerance you want is not available

Sometimes the answer is that the geometry cannot hold what you asked for. The usual fixes, in order of how often they work:

• Split the tolerance across an assembly rather than one part
• Move the tight fit to a metal insert or bushing and let PEEK carry the rest
• Switch to carbon filled stock for stability
• Add a finishing operation after annealing, at the price of a setup
• Accept a matched pair, machined and inspected as a set

Good shops offer these before they quote. If a shop accepts a ±0.01 mm callout on a 200 mm unfilled PEEK part without comment, that is a warning, not a win.

Putting it on the RFQ

Give the grade, the feature that matters, the tolerance and the temperature at which it matters. That is four lines, and it changes the quote more than anything else you can write. What else belongs on a PEEK drawing is in PEEK machining explained.

Have a drawing with a fit you are unsure about? Send it and the shops we match will tell you what they can hold before you commit to it.

Frequently asked questions

Keep reading

• Which Thread Method Works for a PEEK Part: Tap, Mill or Insert
• Specifying Swiss-Type Turned PEEK Parts Without Burrs or Runout