Tolerance callouts on injection molded parts are where a lot of programs quietly overspend. A design engineer used to machined parts will drop ±0.05 mm block tolerances onto a molded housing, the molder quotes to that spec, and the unit price comes back 40% higher than it needed to be. Or worse, the parts come back and half of them fail inspection because nobody caught that the wall thickness makes ±0.05 mm physically impossible.
Here is what to actually specify.
Molded plastic is not machined metal
Injection molded plastic shrinks as it cools. Semi-crystalline resins (nylon, POM, PP) shrink more than amorphous ones (ABS, PC, PS). Shrink rates run 0.4% to 2.5% depending on resin, wall thickness, cooling rate, and fiber content.
That shrink is repeatable within a tool once it is dialed in — but it is not zero, and it is not perfectly uniform. Realistic base tolerances are:
- ±0.1 mm for features under 25 mm on amorphous unfilled resins.
- ±0.2 mm for features up to 100 mm.
- ±0.3–0.5 mm on glass-filled or semi-crystalline resins.
Going tighter is possible but expensive.
Use DIN 16742 (or the SPI table)
Do not invent your own tolerance scheme. Two standards cover this cleanly:
- DIN 16742 — the modern European standard. Two tolerance classes (general and technical) and specific "TG" (tolerance groups) that depend on nominal dimension.
- SPI/DME standard tolerance table — older US practice, still widely used. Distinguishes "commercial" and "fine" tolerances.
Call one of them out on the drawing:
All molded dimensions per DIN 16742, tolerance group TG5, unless otherwise specified.
Then apply tighter callouts only to the specific features that need them — mating features, sealing surfaces, snap fits.
Where tight tolerances actually matter
Molders will hold tighter than the base table on the small number of features where it matters, if you tell them which ones. Typical examples:
- Bearing bores and shaft fits — ±0.05 mm achievable on features under 15 mm with the right gate location.
- Snap fit engagement — ±0.1 mm on the beam and undercut.
- Sealing lands for O-rings — call out surface finish (SPI A2 or B1) in addition to dimensional tolerance.
- Mating features to a PCB or metal chassis — call them out; do not rely on general tolerance.
Everything else — cosmetic outer wall, ribs, boss heights — leave at the general tolerance.
Wall thickness
Wall thickness drives every other decision:
- Ideal wall thickness for most engineering resins: 1.5–3.0 mm.
- Rib thickness: 50–60% of nominal wall.
- Boss OD: 2× nominal wall at the base.
Uniform wall thickness reduces sink, warpage, and cycle time. A part with a 3 mm wall and a 6 mm boss will sink at the boss unless you core it out. The tolerance you can hold gets worse as wall varies.
Draft angle
Draft is not optional:
- 1° minimum on external walls parallel to the pull direction.
- 2–3° on textured surfaces (more draft for coarser texture).
- 0.5° on very small features if the resin releases easily and the tool has adequate ejection.
Zero draft is expensive tooling and slow cycles. Add draft in CAD before you send the RFQ, not after.
Gate location and its effect on tolerance
The gate location determines shrink direction and where the tightest tolerance can actually be held. Features near the gate are tighter; features at the end of fill are looser. If a specific feature must hold ±0.05 mm, discuss gate location with your molder before the tool is cut.
What to send with an RFQ
- 3D model (STEP).
- 2D drawing with:
- Resin, grade, and color.
- Default tolerance callout (DIN 16742 TG or SPI class).
- Tight-tolerance features explicitly dimensioned with individual tolerance.
- SPI mold finish (A1–D3) on cosmetic surfaces.
- Gate location preference or "molder's discretion."
- Annual volume (drives tool class — Class 101, 102, 103, 104, 105).
- Secondary operations (pad print, inserts, ultrasonic weld).
Do that and the quote comes back tight the first time. Send yours here.