Why tolerances should be discussed first
The tolerance on a dimension decides how a part is made, what kind of tool it needs and what it costs. Every tolerance that is tighter than necessary makes the mold more expensive, adds trial rounds and raises the scrap rate. This guide brings together the values you can realistically expect in plastic injection molding, aluminium die casting, gravity die casting and machining.
The values here are commonly used industry guide values and are not binding. The tolerance that can actually be held depends on part geometry, material and mold construction. We review your critical dimensions with you at the quotation stage.
Dimensional tolerances for injection molded plastic parts
Plastic shrinks after it leaves the mold, and the shrinkage rate changes with material, wall thickness and process settings. Semi-crystalline materials (PP, PE, PA, POM) therefore need wider tolerances than amorphous ones (ABS, PC, PMMA). Glass fibre reinforcement reduces shrinkage and allows tighter tolerances.
| Material | 1–20 mm | 21–100 mm | 101–160 mm |
|---|---|---|---|
| ABS, ABS/PC, SAN, PPO | ±0.10 | ±0.15 | ±0.325 |
| PS | ±0.075 | ±0.15 | ±0.305 |
| PP, PE (HDPE/LDPE) | ±0.125 | ±0.17 | ±0.375 |
| PA (nylon), POM | ±0.075 | ±0.16 | ±0.31 |
| PMMA | ±0.075 | ±0.12 | ±0.25 |
| PC, PA 30% GF, PBT 30% GF, PPS 30% GF | ±0.06 | ±0.12 | ±0.24 |
| PC 20% GF | ±0.05 | ±0.10 | ±0.20 |
The table shows the commercial (standard) tolerance class in mm. With a precision mold and tight process control roughly half of these values can be reached, at a higher tooling cost and longer trial phase. GF: glass fibre filled.
Hole diameter tolerances
| Material | Ø 0–3 mm | Ø 3–6 mm | Ø 6–14 mm | Ø 14–40 mm |
|---|---|---|---|---|
| ABS, ABS/PC, SAN | ±0.05 | ±0.05 | ±0.08 | ±0.10 |
| PP, PE | ±0.05 | ±0.08 | ±0.10 | ±0.15 |
| PA, POM | ±0.05 | ±0.08 | ±0.08 | ±0.13 |
| PMMA | ±0.08 | ±0.08 | ±0.10 | ±0.13 |
| PC and glass filled grades | ±0.05 | ±0.05 | ±0.08 | ±0.08 |
Flatness and straightness
Warpage comes from the material shrinking differently along and across the flow direction; it is more pronounced in fibre filled materials and in parts with varying wall thickness. Mold design, gate position and process control reduce the effect but cannot remove it completely.
| Material | 0–100 mm | 101–160 mm |
|---|---|---|
| ABS, ABS/PC, SAN, PPO | 0.38 | 0.80 |
| PA, POM | 0.30 | 0.50 |
| PS | 0.25 | 0.38 |
| PMMA | 0.18 | 0.33 |
| PC and glass filled grades | 0.15 | 0.20 |
| PP, PE | 0.85 | 1.50 |
To see warpage risk before the mold is built we run a mold flow analysis.
Tolerances for aluminium high pressure die castings
In die casting the tolerance is calculated from the length of the dimension: a basic value for the first 25 mm plus an additional value for every further 25 mm.
| Class | First 25 mm | Each additional 25 mm |
|---|---|---|
| Standard | ±0.25 mm | ±0.025 mm |
| Precision | ±0.05 mm | ±0.025 mm |
Example: a 125 mm dimension in the standard class gets ±0.25 + 4 × 0.025 = ±0.35 mm. Tighter tolerances mean the die needs maintenance sooner, because dimensions drift as the die wears.
Dimensions across the parting line
Dimensions formed between the two die halves receive an extra plus tolerance based on the projected area of the casting at the parting plane. A fully closed die has zero separation, so this addition is plus only.
| Projected area | Additional tolerance for aluminium |
|---|---|
| up to 65 cm² | +0.14 mm |
| 65–130 cm² | +0.165 mm |
| 130–325 cm² | +0.19 mm |
| 325–650 cm² | +0.30 mm |
| 650–1300 cm² | +0.46 mm |
| 1300–1950 cm² | +0.61 mm |
Draft
The draft angle a casting needs gets smaller as the feature gets deeper. Typical values for inside walls in aluminium:
| Depth | Approximate draft angle |
|---|---|
| 2.5 mm | 6° |
| 25 mm | 1.9° |
| 127 mm | 0.85° |
Outside walls need about half of these values, because the casting shrinks away from the cavity walls but onto the cores.
As-cast surface classes
| Class | As-cast surface | Typical use |
|---|---|---|
| 1 – Utility | No cosmetic requirement; cold shuts and rub marks acceptable | Used as cast or with protective coating |
| 2 – Functional | Marks that can be removed by spot polishing or covered by heavy paint are acceptable | Painted, lacquered or plated parts |
| 3 – Commercial | Slight, removable surface imperfections acceptable | Structural parts, electrostatic painting |
| 4 – Consumer | No objectionable imperfections | Decorative parts |
| 5 – Superior | Roughness value specified on the drawing for limited areas | O-ring seats and gasket faces |
Practical limits in casting design
- Keep wall thickness as uniform as possible; the thickest section should not exceed twice the thinnest.
- Use fillet radii of at least 1.5 mm and corner radii of at least 0.5 mm.
- For cored holes under 12.5 mm diameter keep depth below 4 × diameter; for larger holes below 10 × diameter.
- Raised lettering is cheaper and kinder to the die than recessed lettering; keep line width at 0.25 mm or more and draft above 10°.
- Ejector pin marks may be raised or depressed by about 0.4 mm; tell us which faces are visible so we keep ejectors away from them.
Tolerances for gravity die (permanent mold) castings
Gravity die castings have wider tolerances than high pressure die castings; in series production grades DCTG 6–8 to ISO 8062-3 are usual. Faces that need tighter tolerances are machined after casting.
Tolerances in machining
Dimensions without an individual tolerance on the drawing follow the ISO 2768 general tolerances, usually class “m – medium”. Fits are specified to ISO 286.
Five rules for setting tolerances
- Give tight tolerances only to dimensions with a function: fits, sealing faces, assembly datums.
- Keep critical dimensions in one mold half where possible; dimensions crossing the parting line or a moving core are always wider.
- In plastics, changing the material changes the tolerance; a mold is cut for the shrinkage of one material.
- State the measuring condition: plastic parts keep changing size after molding and nylon grows as it absorbs moisture.
- Where a casting cannot hold the tolerance, machine it; leave machining stock only on the faces that need it.
Sources: NADCA “Product Specification Standards for Die Castings”; ISO 8062-3; ISO 2768-1; commercial tolerance tables commonly used in plastic injection molding.