Every dimension on your drawing is a promise about a plastic part that will be moulded hot and will shrink as it cools. If the shrinkage number used to cut the cavity is wrong, the part arrives 0.2–0.4 mm off nominal — perfectly moulded, perfectly useless. And if the tolerance block was copied from a machined metal part, no mold on earth will hold it.
This guide gives you the practical numbers: shrinkage rates by material, how to convert them into cavity dimensions, what DIN 16901 and ISO 20457 tolerance classes mean, what silicone and rubber do differently, and how to write a callout a toolmaker can hold without quietly adding 30% to your tooling price.
Why shrinkage decides your tolerance
Plastic shrinks because its molecules pack tighter as they cool from melt temperature to room temperature. Amorphous materials (ABS, PC, PS) shrink modestly and fairly evenly. Semi-crystalline materials (PP, PE, PA, POM) shrink much more, because the crystal regions that form during cooling take up less volume — and the amount depends on how fast you cool, at what pressure you pack, and which direction the melt flowed.
Three consequences follow, and they explain most tolerance disputes:
- The tool is not the part. A cavity cut to 100.00 mm produces roughly a 98 mm part in PP.
- Shrinkage is a range, not a number. Suppliers publish 1.5–2.5% for PP, not 2.0%, and your run lands somewhere inside that band.
- Size amplifies error. A 0.3% uncertainty is 0.03 mm at 10 mm nominal and 0.6 mm at 200 mm — which is exactly why the standards widen tolerance with size.
Shrinkage rates by material
Values below are typical mould shrinkage measured per ISO 294-4 (or ASTM D955) on standard test bars. Treat them as a starting point for quoting and DFM, never as a substitute for the resin supplier's own datasheet for your specific grade.
| Material | Type | Typical shrinkage | Tolerance difficulty |
|---|---|---|---|
| ABS | Amorphous | 0.4 – 0.7% | Low — good baseline |
| PC / PC-ABS | Amorphous | 0.5 – 0.7% | Low — needs good drying |
| PMMA | Amorphous | 0.3 – 0.6% | Low, but optical defects dominate |
| PA66 (unfilled) | Semi-crystalline | 1.0 – 1.5% | Medium — moisture sensitive |
| PA66-GF30 | Semi-crystalline + GF | 0.3 – 0.6% | Medium — anisotropic, warps |
| POM | Semi-crystalline | 1.8 – 2.5% | High, but very stable after moulding |
| PP (unfilled) | Semi-crystalline | 1.2 – 2.5% | High — hardest common material for tight work |
| PP + 20–30% talc / GF | Semi-crystalline + filler | 0.3 – 1.2% | Medium — much better than unfilled |
| PE-HD / PE-LD | Semi-crystalline | 1.5 – 3.5% | High — soft, creep-prone |
| PBT / PET (unfilled) | Semi-crystalline | 1.5 – 2.0% | Medium |
| PBT-GF30 | Semi-crystalline + GF | 0.3 – 0.5% | Medium — flow-direction difference matters |
| TPE / TPU | Soft, semi-crystalline | 1.5 – 3.0% | High — soft parts deform on measurement |
From shrinkage to cavity size: the actual calculation
Toolmakers do not guess. They scale the cavity by the material's shrinkage. The relationship is simple:
Cavity dimension = Part dimension ÷ (1 − shrinkage), and the reverse, Part dimension = Cavity dimension × (1 − shrinkage).
Worked example — a 120 mm long PP housing, shrinkage 1.8% (mid-band of a 1.5–2.1% grade):
- Cavity length = 120 ÷ (1 − 0.018) = 122.20 mm
- If the real shrinkage drifts to 1.5%: part = 122.20 × 0.985 = 120.37 mm (+0.37 mm)
- If it drifts to 2.1%: part = 122.20 × 0.979 = 119.63 mm (−0.37 mm)
So a 30-year-old rule of thumb ("PP shrinks 2%") hands you ±0.37 mm before you have even cut steel. That is why a ±0.1 mm callout on a 120 mm PP part is a conversation, not a specification: it can only be met by rebuilding the cavity after T1 measurement, or by choosing a filled grade instead.
Anisotropy: shrinkage is not the same in every direction
In filled and semi-crystalline materials, shrinkage measured along the melt flow is typically 0.2–0.8 percentage points lower than shrinkage across the flow. Glass fibres align with the flow and hold that direction open; the cross-flow direction then has to absorb more contraction.
The result is differential shrinkage — the physical cause of warpage and of the classic complaint "the length is fine but it bows 0.8 mm". Practical responses, in order of cost:
- Move the gate so the flow path is symmetric on both sides of the part
- Balance cooling so both faces reach ejection temperature together (see cooling system design)
- Add ribs or a slight counter-camber in the cavity so the part straightens after shrinkage
- Accept a straightness callout instead of a dimensional callout, and control it with a checking fixture
Every one of these should be identified during DFM review, before the cavity is cut — not after T1 samples come back bent.
Tolerance classes: what DIN 16901 and ISO 20457 give you
Two standards cover the same idea. DIN 16901 defines general tolerances for moulded parts through tolerance series 110–160, with the permitted deviation growing as the nominal dimension grows. ISO 20457 (with the Chinese GB/T 14486 aligned to it) groups materials into shrinkage categories MT1–MT7 and offers grades A (precision), B (standard) and C (coarse).
The important part for a buyer is the shape of the curve, not the table number: tolerance is a function of nominal size × material shrinkage class. The table below gives achievable tolerances in normal production for a low-shrinkage material such as ABS or PC; wider grades scale up as noted underneath.
| Nominal size (mm) | Standard ± (mm) | Technical ± (mm) | Precision ± (mm) |
|---|---|---|---|
| 1 – 3 | 0.10 | 0.06 | 0.04 |
| 3 – 6 | 0.12 | 0.08 | 0.05 |
| 6 – 10 | 0.14 | 0.10 | 0.06 |
| 10 – 18 | 0.18 | 0.12 | 0.07 |
| 18 – 30 | 0.21 | 0.14 | 0.09 |
| 30 – 50 | 0.25 | 0.18 | 0.11 |
| 50 – 80 | 0.30 | 0.22 | 0.14 |
| 80 – 120 | 0.40 | 0.28 | 0.18 |
| 120 – 180 | 0.50 | 0.35 | 0.22 |
| 180 – 250 | 0.65 | 0.45 | 0.28 |
Multipliers on the standard column for other material classes: glass-filled grades ≈ ×1.1; unfilled PA, PBT and POM ≈ ×1.3; filled PP or PE-HD ≈ ×1.5; unfilled PP or PE-LD ≈ ×1.8; soft TPE ≈ ×2.0. The same 100 mm dimension is a comfortable 0.40 mm in ABS and a genuinely difficult 0.15 mm in unfilled PP — physics, not supplier skill.
Silicone and rubber: different rules
Silicone parts are frequently quoted on plastic tolerances and then fail inspection, because rubber moves far more than thermoplastic after demoulding.
- HCR compression moulding: shrinkage typically 2–4%, driven by cure temperature, compound hardness and part thickness. Thick sections shrink more than thin ones because the core cures later.
- LSR injection moulding: 1.5–3% at the tool, plus post-cure shrinkage of roughly 0.3–1.5% in the hours and days after demoulding. Measuring LSR parts straight off the press is the single most common measurement error in silicone projects.
- Standards: rubber dimensional tolerances are normally specified per ISO 3302-1 classes M1–M4, not by metal tolerance blocks. A 50 mm silicone gasket at class M2 carries roughly ±0.4 mm; M1 tighter, M3/M4 much wider.
Practical rule: for silicone, state the measuring condition on the drawing — hours after demoulding, temperature, post-cured or not — alongside the tolerance. Without it, two inspectors will disagree and both will be right.
What actually drives the tolerance you can hold
Material sets the floor, but five tool and process decisions decide whether you reach it:
- Tool rigidity and steel choice. Thin cavities deflect under injection pressure. Precision class usually means hardened core/cavity (H13 or hardened P20) rather than a pre-hardened block — which is a real cost step.
- Cooling balance. Uneven mould temperature is uneven shrinkage. Half of all "impossible tolerance" cases are cooling problems wearing a tolerance costume.
- Gate location and packing. Gate far from a dimension means that dimension packs less and shrinks more. Gate position is a tolerance decision.
- Cavitation. Multi-cavity tools need matched cavity steel, and each cavity needs its own correction after T1. Four cavities mean four sets of dimension corrections, not one.
- Process window and measurement. Precision parts need a defined process window, conditioned parts, and a CMM or gauge plan agreed before T1 — otherwise acceptance becomes opinion.
What a tight tolerance costs
Tightening every dimension "just to be safe" is the most expensive habit in plastic part design. Moving a tool from standard to precision class typically adds:
| Cost driver | Typical impact |
|---|---|
| Hardened steel and stress-relieved cavity inserts | +10 – 20% on tool cost |
| Slower EDM / high-speed milling, more polishing | +5 – 15% on tool cost |
| Extra trial loops (T1 measurement → steel correction → T2) | +1 – 3 weeks schedule |
| CMM inspection and capability study per cavity | +per-part QC cost, sometimes 2–5% of piece price |
| Higher scrap rate in the first months of production | 3 – 10% of parts at ramp-up |
The efficient approach is critical dimensioning: mark the few dimensions that touch a mating part, a seal or an assembly stack, hold those to precision class, give everything else the standard block. Buyers who do this usually cut 15–30% off the tooling quote without changing function at all.
How to write the tolerance block on your drawing
- Start from the material, not the number: pick the resin first, read its datasheet shrinkage range, then set the tolerance band it can physically support.
- Use one general tolerance block (per DIN 16901 or ISO 20457 grade) plus a short list of individually toleranced critical dimensions — never a uniform ±0.05 mm on every feature.
- Give tolerances per feature type: bores and bosses hold tighter than long linear dimensions; features across the parting line or formed by sliders carry extra variation and need wider bands.
- For silicone and rubber, cite ISO 3302-1 class and define the measuring condition.
- Agree the datum scheme with the toolmaker before T1, and state which dimensions are measured on a CMM versus a gauge.
- Allow one steel-correction loop. Every first tool needs it; a supplier promising zero corrections is either very experienced or not planning to measure.
RFQ checklist: tolerance and shrinkage
- ☐ Resin grade and supplier datasheet shrinkage range attached to the RFQ
- ☐ General tolerance standard chosen (DIN 16901 / ISO 20457 grade)
- ☐ Critical dimensions flagged, and only those
- ☐ Nominal size of the largest critical dimension noted — it sets the achievable band
- ☐ Warpage / flatness requirements stated separately from dimensions
- ☐ Gate position agreed (it changes which dimensions shrink more)
- ☐ Cavity count fixed, with a plan for per-cavity correction after T1
- ☐ Measurement method and conditioning time defined for rubber parts
- ☐ One steel-correction loop allowed in the delivery schedule
- ☐ Capability expectation agreed (what Cpk, on which dimensions, for how many shots)
Get the shrinkage assumption checked before steel is cut
Precimold designs and builds injection moulds for plastic and silicone parts up to 2 m × 1.6 m, and reviews shrinkage and tolerance assumptions on every drawing before quoting. Send us your 3D model, resin grade and the dimensions that actually matter for assembly — we will come back with the shrinkage band we would cut to, the tolerance each feature can realistically hold, and the tooling cost difference between standard and precision class. We reply within 12 hours.
Send your drawing for a tolerance review
Upload the 3D model and name your critical dimensions — we will return the shrinkage assumption, achievable tolerance per feature, and the cost impact of tightening only what needs it.
Request a quote