Plastic Part Tolerance Standards: ISO 20457 and DIN 16742

Metal tolerances are a solved problem: you cut to size and the tolerance holds. Molded plastic is different. The part shrinks by 0.4–2.5% as it cools, that shrinkage varies with wall thickness, flow direction, gate location, fiber orientation and mold temperature, and it keeps changing for hours after ejection.

Figure 1. Plastic Part Tolerance Standards: ISO 20457 and DIN 16742.

Applying a general engineering tolerance table to a molded part is the fastest way to generate a stream of unnecessary rejections and expensive tooling changes. This guide explains the plastic-specific standards and how to apply them so that the tolerances you put on a drawing are tolerances the process can actually hold.

1. Why Plastic Tolerances Are Different

Four effects make molded dimensions move:

1. Shrinkage. Every resin has a nominal shrink rate, but the actual rate depends on the local cooling and packing conditions. A rib cools faster than an adjacent wall and shrinks less.
2. Anisotropy. Glass- and carbon-filled materials shrink roughly half as much along the fiber direction as across it. A single nominal shrink figure cannot represent both.
3. Post-mold shrinkage. Semi-crystalline resins such as POM, PA and PP continue to shrink after ejection, particularly if the part absorbs moisture or anneals. This can continue for days.
4. Process variation. Mold temperature, hold pressure and cycle time all shift shrinkage. A ±5 °C mold temperature change can move a dimension by 0.05 mm on a 100 mm part.

The result is that plastic tolerances are graded by material and by the size of the dimension, not applied as a flat ±0.1 mm.

2. The Standards Landscape

Practical position: for new drawings, specify ISO 20457 and reference the tolerance grade. Where a customer or an existing tool requires DIN 16742, the grades and the material groups correspond closely, so a grade such as 130 transfers with minimal rework. If you work with Chinese toolmakers, expect GB/T 14486 to appear and confirm the grade mapping explicitly.

3. How the Grading System Works

The standard works on two axes:

Axis 1 — Material group, based on mold shrinkage and its variability:

The material group sets the baseline tolerance, because a semi-crystalline resin with 2% shrink and high variability simply cannot hold the same tolerance as an amorphous resin with 0.5%.

Axis 2 — Tolerance grade, a number where larger = coarser. Grades run from roughly 100 (precision) to 500+ (coarse). For most molded parts:

Key principle: tolerance is graded per dimension, not per drawing. A single part can legitimately have a grade-130 mating dimension and a grade-200 overall length. Grading the whole drawing to a single tight grade is what makes plastic parts expensive.

4. Tolerance Value Scales With Size

Tolerance is not a fixed band; it grows with the dimension. This is fundamental and often ignored.

A useful working model, consistent with the standards' structure:

> Tolerance ≈ (k × L^0.4) × grade factor

where L is the dimension length in mm and k depends on the material group. The exponent around 0.4 means tolerance grows much more slowly than the dimension itself, but it does grow.

Practical consequences:

• A 5 mm feature on a grade-140 amorphous part might hold ±0.05 mm.
• The same grade on a 200 mm dimension might only hold ±0.35 mm.
• Asking for ±0.05 mm on a 200 mm molded dimension is asking for something the process cannot deliver — the tool will be cut, the parts will be rejected, and the argument will be about the material rather than the specification.

Rule of thumb: if a tolerance is tighter than roughly 0.1% of the dimension on a mold-direct dimension, challenge it. Either the dimension needs a design change (move the tolerance to a machined feature or a controlled datum) or the requirement is genuinely wrong.

5. Which Dimensions to Tolerance — and Which Not

Not every dimension deserves a tolerance, and the most common cause of scrap is a tolerance applied to a dimension that should never have carried one.

Do not put tight tolerances on:

• Dimensions across a parting line. The two halves of the tool move and wear independently. Give parting-line dimensions a coarser grade or move them off the parting line.
• Dimensions influenced by two independently moving tool components — e.g. across a slide shut-off and the parting line.
• Wall thickness as a "dimension". Specify a nominal with a process capability note, not a tight bilateral tolerance. Wall thickness variation is a molding outcome.
• Dimensions to a free-form surface or a converted spline. Datum them properly or tolerance only the functional points.
• Overall length on a long, thin part. Thermal and shrinkage variation accumulates. Control the functional distance, not the outer envelope.
• Any dimension that the part's function does not actually depend on. Challenge every tolerance on the drawing: "what fails if this is out?" If nothing fails, loosen it.

Do put tight tolerances on:

• Mating and assembly interfaces — where the part has to fit another part or a fixture.
• Hole positions for fasteners, usually as positional tolerance rather than ± on coordinates.
• Functional dimensions — sealing surfaces, connector pitch, optical centers.
• Datums themselves, which should be functional molding features, not arbitrary edges.

6. Datum Strategy and GD&T for Molded Parts

Geometric dimensioning and tolerancing is more useful for plastic parts than for machined parts, not less — but only if the datums are chosen sensibly.

Datum selection rules:

• Choose datums that correspond to mold-relevant features — a shut-off surface, a cavity-formed face, a boss center.
• Establish the primary datum as a large, flat, molded surface. This is the surface that will also be the fixturing surface for inspection.
• Do not use a parting-line edge as a primary datum; it is the least repeatable feature on the part.
• For mating assemblies, use functional datums (the surfaces that actually locate the mating part) rather than datum targets chosen for convenience.

Positional tolerancing in practice:

• Use positional tolerance with MMC for hole patterns where the fastener has a fixed size, so bonus tolerance is available.
• Use profile tolerance for complex surfaces; it is the only practical way to control a free-form surface.
• Use flatness and straightness rather than tight ± on individual points where the function is flatness — this is far more achievable on a molded part.

7. Achieving the Tolerance You Specified

Once the drawing is written, three things decide whether the parts hold it:

• Tool design. Gate location, cooling uniformity and packing balance determine whether dimensions repeat shot to shot. A well-cooled, balanced tool holds grade 140 almost automatically.
• Mold qualification process. Run a capability study (Cpk) on critical dimensions from a controlled process, at minimum 30 samples. Do not accept a "first article matches drawing" as evidence of capability — first articles are often molded on an artificially optimized process.
• Post-mold control. For semi-crystalline and moisture-absorbing resins, specify conditioning (e.g. moisture conditioning for PA, annealing for some grades) before dimensional inspection, and define the conditioning window on the drawing. Measuring a PA part 10 minutes after molding and again 48 hours later gives two different answers, and both are "correct".

Shrinkage compensation: work with your moldmaker to cut steel based on measured molded shrinkage from a trial tool, not on the resin supplier's nominal data sheet range. This single step resolves the majority of dimensional disputes on new tools.

Figure 2. Quick reference: the key checks and reference values from this guide.

8. Specification Checklist

• [ ] Customer-specific tolerance standard checked before defaulting to ISO 20457
• [ ] Material group identified from the resin's shrink class
• [ ] Tolerance grade assigned per dimension, not per drawing
• [ ] No mold-direct dimension tighter than roughly 0.1% of its length
• [ ] Parting-line and cross-slide dimensions given coarser tolerance
• [ ] Wall thickness specified as nominal with process note, not tight bilateral
• [ ] Functional datums defined; primary datum is a large molded surface
• [ ] Non-functional dimensions deliberately loosened and documented
• [ ] Positional and profile tolerancing used instead of coordinate ± where appropriate
• [ ] Conditioning window specified for hygroscopic or semi-crystalline resins
• [ ] Cpk requirement stated for critical dimensions (e.g. Cpk ≥ 1.33)
• [ ] Steel cutting based on measured trial shrinkage, not data sheet nominal

Conclusion

The value of ISO 20457 and DIN 16742 is not the tables — it is the discipline of connecting every tolerance to a material group, a dimension size and a molding process that can actually deliver it. Grade the dimensions individually, keep tight tolerance where the function demands it, loosen it everywhere else, and choose datums that the mold can actually produce repeatedly.

Send us your drawing and we will flag the tolerances that the molding process cannot hold, and propose alternatives, before the tool is cut.