Clearances for 3D-Printed Parts That Have to Move

A pin modelled at exactly 5 mm will not turn in a hole modelled at exactly 5 mm. It will not even go in. Printed holes come out undersized and printed pegs come out oversized, and those two errors add rather than cancel. The gap that fixes it is not a property of the design — it belongs to the printer, the material and the profile, which is why it has to be measured once rather than looked up forever.

Four effects push a printed dimension away from its nominal value, and on a hole-and-pin pair they conspire.

The bead is wider than the path. Molten polymer leaving a nozzle swells, and the slicer squashes it against the layer below. The deposited line is wider than the toolpath it followed. On an outside edge that adds material outward; on the inside of a hole it adds material inward. The hole shrinks and the pin grows.

Corners overshoot. The nozzle cannot turn instantly. On a small hole the path is a tight polygon, and the extruder is still catching up as the direction changes, which leaves the corners slightly full. Small holes suffer far more than large ones — proportionally, a 3 mm hole loses much more of its diameter than a 30 mm one.

The first layer spreads. Squish flattens the bottom layer outward. A peg is widest at its base, a hole is tightest there, and if the mating surface is near the plate that is the dimension that governs.

Everything contracts on cooling. Not uniformly, and not equally in every direction, which is why a long part and a short part in the same material do not scale by the same factor.

None of this makes a printer inaccurate. It makes it consistently offset, which is a much better problem: an offset can be measured once and designed around.

Most published clearance figures are diametral: the difference between hole diameter and pin diameter. A 0.4 mm diametral clearance means the hole is 0.4 mm larger across, which leaves 0.2 mm of air on each side.

That factor of two is the most common error in printed assemblies. Applying a 0.4 mm number as a per-side gap gives 0.8 mm of total slop, and the hinge that was meant to feel solid rattles. Applying a per-side figure diametrally gives half the intended gap, and the pin will not go in.

The rule to carry: a clearance applied to a radius is half the clearance applied to a diameter. Before using any number from any source, including this article, establish which one it is.

The same confusion appears in a subtler form when one variable drives two different kinds of fit. A hinge with a pin through a knuckle has a radial gap around the pin and an axial gap between knuckles. If both are driven from one clearance value, they are almost certainly not receiving the same amount — one is typically half the other. That is fine as long as it is deliberate. It is a problem when a value calibrated until the pin turns smoothly silently delivers twice that as end float.

Engineering fits have formal definitions for machined parts. Printed parts need the same categories with coarser numbers, because the process variation is larger than the tolerance bands those standards assume.

Table: Starting diametral clearances for FDM at a 0.4 mm nozzle. First-print values to calibrate from, not specifications.

Three qualifications matter more than the numbers.

Bigger features need more. These figures suit features in the 3 to 20 mm range. A 60 mm bore needs a larger absolute clearance because the same percentage error is a larger absolute error, and because contraction scales with length.

Print-in-place is a different constraint. The gap between two parts printed together must be large enough that the slicer does not bridge it — which usually means at least one nozzle diameter, and in practice a little more. Below that the parts fuse and the mechanism is a solid block. This is a slicer question, not a fit question.

Material changes the answer. PETG and TPU deposit wider and stickier than PLA, and a clearance calibrated in PLA will often bind in PETG. Treat the calibration as belonging to a material as well as a machine.

Every table in every article on this subject is a guess about someone else's printer. Twenty minutes of printing replaces it with a fact about yours.

The method is old and it is what standards bodies do at a larger scale: build one artefact that exercises the feature you care about across a range, measure the result, and record the offset as a property of the process.^[1] A feature-based approach to designing such artefacts — choosing which features to include based on what actually needs characterising — is the formal version of the same idea.^[2]

For clearances, the coupon is simple:

1. Model one plate with a row of holes, all the same nominal diameter, stepping the clearance from 0.1 mm to 0.8 mm in 0.1 mm increments. Label each one in the model so the printed part is self-documenting.
2. Model a matching set of pins, or use a single pin and a row of holes.
3. Print it in the orientation and profile the real part will use. Orientation matters: a hole printed vertically and a hole printed horizontally are not the same hole.
4. Try each fit by hand. The first that moves freely is the free-running clearance. The last that assembles with effort is the press fit.
5. Write the numbers down as part of the printer profile, next to flow rate and first-layer height.

Repeat per material, not per part. The result is a small table that is worth more than anything published, because it describes the machine that will actually do the work.

This is also how the rigorous literature approaches the problem: characterise the process capability first, then predict whether an assembly will go together, rather than assuming nominal dimensions and hoping.^[3] There is even work costing tolerances for extrusion processes specifically — tightening a fit is not free, and past a point the extra print time and scrap outweigh the benefit.^[4]

A fit that depends on hitting a dimension exactly is fragile. Several constructions make the same assembly tolerant of being slightly wrong.

Chamfer every lead-in. A 45 degree chamfer on the mouth of a hole and the end of a pin turns an interference into a guided entry. This single change rescues more marginal fits than any clearance adjustment.

Contact on three points, not a full circle. A pin in a round hole must match all the way round. A pin in a slot, or a shaft on three pads, only has to match where the pads are, and the errors elsewhere stop mattering.

Let something flex. A short cantilever or a thin web absorbs a tenth of a millimetre without complaint. Compliance is cheap in printed plastic and it is the reason snap fits tolerate wide process variation.

Split the tolerance across the joint. If two mating parts each carry half the clearance, each one is a less demanding print than one part carrying all of it.

Prefer adjustment to precision. A slot instead of a hole, a screw instead of a press fit, a shim pocket: any of these converts a dimension that has to be right into one that can be corrected after printing.

The physical explanations in this article are well established. The numbers are not, and it is worth being plain about the difference.

There is serious published work on geometric capability and assemblability in additive manufacturing, and on the cost of tightening a tolerance in extrusion processes. Most of it targets metal powder-bed fusion or industrial machines, uses measurement equipment a hobbyist does not have, and reports process capability rather than design rules. The specific bands that circulate for desktop FDM — 0.2 mm for a close fit, 0.5 mm for free running — come from printer manufacturers, service bureaux and accumulated forum practice.

That is not a dismissal. Those sources represent an enormous amount of real printing, and the numbers are broadly right for a broadly typical machine. But there is no peer-reviewed table to appeal to, the tolerance a given desktop printer can hold varies more between machines than most published figures admit, and anyone quoting these bands with confidence is quoting practice rather than evidence.

The practical response is the same one the standards literature arrives at from the other direction: measure your own process. The coupon above is the smallest version of that, and it outranks every published band, including the one in this article.

The other two design rules in this series arrive at the same place — a number that has to be measured rather than looked up. How Thick Should 3D-Printed Walls Be? is about the nozzle setting the wall, not the design. The 45° Overhang Rule, and When It Is Wrong is about how far a layer can lean before the one below stops holding it up. Both come with a coupon to measure it on your own machine.

For a worked hinge that carries its clearance as a calibrated variable rather than a typed number, see Fits, Clearances, and Tolerances for Customized 3D Prints.

For threaded pairs, where clearance also has to account for helix phase before the parts will mesh, see Threads and Snap Fits That Print. For recording a calibration so it survives the next order rather than being rediscovered, see Versioned Production: Presets, Reorders, and Change Control.