Views: 0 Author: Abery Engineering Team Publish Time: 2026-10-08 Origin: Abery Mold
The realistic tolerance window for injection molding is ±0.05 mm on small features in stable engineering resins for precision work, and ±0.1–0.3 mm as the standard commercial range — and any blanket tolerance tighter than ±0.05 mm on a drawing is usually a signal the tolerances were copied, not engineered.
Below is the working tolerance reference we quote against, organized the way parts actually behave: by feature size and material family, because shrinkage — not the machine — sets the floor.
Working values for well-designed molds with controlled process (aligned to DIN 16742 / ISO 20457 "standard" and "fine" groups):
Nominal Feature Size | Standard Commercial (Group 2) | Precision / Fine (Group 1) | Below This = Machining Territory |
|---|---|---|---|
0–10 mm | ±0.10 mm | ±0.05 mm | < ±0.03 mm |
10–30 mm | ±0.15 mm | ±0.08 mm | < ±0.05 mm |
30–100 mm | ±0.20 mm | ±0.10 mm | < ±0.08 mm |
100–300 mm | ±0.30 mm | ±0.15 mm | < ±0.10 mm |
300+ mm | ±0.05% of dimension | ±0.03% of dimension | consult in DFM |
How to read this table: the "standard" column is what any competent shop should hold without special pricing. The "precision" column is achievable but should be applied selectively — to mating interfaces, bearing seats, snap fits. Everything below the third column belongs on a machining center after molding, or in metal, not negotiated into a molding price.
Tolerance achievability starts with how much the resin shrinks and how consistently:
Resin Family | Shrinkage (typical) | Tolerance Achievability | Notes |
|---|---|---|---|
ABS, PS, SAN | 0.4–0.7% | Good | Stable, low moisture sensitivity |
PC | 0.5–0.7% | Good | Needs drying; stress issues if abused |
PA6 / PA66 (nylon) | 1.0–1.8% | Moderate | Post-molding moisture absorption moves dimensions for days |
POM (acetal) | 1.8–2.5% | Moderate | High shrink, moldable to spec with tight process window |
PP, PE | 1.5–2.5% | Poorest | Depressed center shrink; tight tolerances on large parts are a fight |
Glass-filled (GF20–GF33) | 0.2–0.6% | Very good along flow | Anisotropic — tighter parallel to flow direction |
The direct takeaway: if your drawing needs ±0.05 mm on a 60 mm feature, almost any unfilled amorphous resin gets there; if it's nylon or polypropylene at 200 mm, ±0.05 mm is a conversation about moisture conditioning and gate design, not a quote line.
Each step tighter compounds cost in three places at once:
Tightening From... To... | Mold Cost | Process Cost | Inspection Cost |
|---|---|---|---|
Group 2 → Group 1 (few features) | +10–20% (hardened steel, precision grinding) | Drying discipline, narrower process window | Periodic CMM checks |
Group 1 blanket across drawing | +30–50% | Slower cycles, higher scrap sensitivity | 100% inspection or per-lot CMM |
Below ±0.05 mm anywhere | Post-mold machining may be cheaper | — | SPC + MSA studies required |
A 4-cavity PA66-GF20 electronic connector we run holds ±0.03 mm on critical pins — but the drawing only calls that class on the mating geometry; the rest runs standard. That selective callout is why the mold was affordable and the parts pass first article on the first try.
Blanket title-block tolerances (±0.05 everywhere): cost without function. Fix by marking only the 2–5 dimensions that genuinely interface with something.
Tolerancing a draft-affected surface as a true wall position: draft angle consumes tolerance budget; dimension the datum end, accept the draft.
Ignoring nylon's moisture growth: a PA66 part measured dry-as-molded will read differently after a week at 50% RH. If the assembly tolerance is tight, specify conditioning protocol in the drawing notes.
Tolerances degrade as the mold wears — a Class 104 mold holding ±0.1 mm at shot 10,000 may not at shot 90,000. If your program needs Group 1 tolerances over a multi-year life, that decision points back to hardened steel (SPI Class 101/102) at the quoting stage, not to a tighter process on a soft mold. See Injection Molding Standards: SPI Classes & Tolerance Grades for the class-by-class breakdown.
Mark up your drawing like this and any serious molder's quote gets sharper:
Highlight the dimensions that interface with mating parts — candidate for Group 1
Note which resin (and whether glass-filled)
Flag any dimension on a drafted surface
If nylon/POM: note the conditioning environment the dimension applies at
Remove or loosen any holdover title-block tolerances on non-functional features
Send us the marked-up drawing — our DFM comes back with per-dimension feasibility (holdable / tight-but-doable / needs redesign) inside 24 hours. → Get a tolerance review with your quote
Related reading: Injection Molding Standards Explained · ISO 13485 Medical Injection Molding: What Buyers Must Verify
Written by the Abery engineering team — Shenzhen-based custom injection mold and molding manufacturer, IATF 16949:2016 certified.
