Front page / What tolerances can injection moulding hold?
What tolerances can injection moulding hold?
Injection moulding has no single tolerance: Komaspec explains that general tolerances come from DIN ISO 20457 tolerance groups indexed to size, while Fictiv's published tables show values that widen with part size and change with the resin.
For a first part, the useful question is not "how tight can moulding go?" but "which few dimensions need to be tight, and what will the rest cost me if I over-specify them?" This article sets out the published figures, what drives them, and a practical way to tolerance a drawing.
What the published figures say
Three sources give quite different kinds of number, so it helps to see them side by side.
| Source | What it publishes | Figure |
|---|---|---|
| Protolabs | Typical machining tolerance | ±0.003 in (0.08 mm) |
| Protolabs | Resin tolerance added on top | no less than ±0.002 in/in (0.002 mm/mm), and can be greater |
| Fictiv | Typical for non-critical consumer parts | ±0.1 mm |
| Fictiv | Typical for tighter work such as medical parts | ±0.025 mm |
| Fictiv | Typical mould machining | ±0.127 mm, with tighter moulds at ±0.0508 mm or ±0.0254 mm |
The two mould-machining figures do not agree: Protolabs quotes its own typical value, while Fictiv describes a general industry figure. Neither is a promise for your part. The Protolabs resin allowance is the more useful planning number, because it scales with size. As simple arithmetic on that figure, a 100 mm dimension would carry a resin allowance of at least ±0.2 mm before the machining tolerance is added.
Commercial versus fine tolerances
Fictiv publishes tables that it describes as typical values from the SPI (now the Plastics Industry Association), split into "commercial" and "fine" columns. Commercial tolerances use lower-cost moulds and produce cheaper parts; fine (precision) tolerances need a tighter tool and process, so both the mould and every part cost more. Fictiv says to discuss the values with your mould maker. A selection of its dimensional values (mm, by nominal size) is shown below.
| Resin | Commercial, 1 to 20 mm | Commercial, 21 to 100 mm | Commercial, 101 to 160 mm | Fine, 1 to 20 mm | Fine, 21 to 100 mm |
|---|---|---|---|---|---|
| ABS | 0.100 | 0.150 | 0.325 | 0.050 | 0.100 |
| Polypropylene | 0.125 | 0.170 | 0.375 | 0.075 | 0.110 |
| Acetal (POM) | 0.075 | 0.160 | 0.310 | 0.030 | 0.130 |
| 30 % glass-filled nylon | 0.060 | 0.120 | 0.240 | 0.030 | 0.100 |
Fictiv adds a further allowance for each 20 mm above 160 mm (0.080 mm for ABS, 0.100 mm for polypropylene). Its flatness table shows the same pattern more sharply: for a 0 to 100 mm span, ABS is listed at 0.380 mm commercial and 0.250 mm fine, while polypropylene is listed at 0.850 mm commercial and 0.500 mm fine.
Two things stand out. Tolerances widen considerably as a dimension moves from the smallest to the largest size band (ABS goes from 0.100 to 0.325 mm commercial), and polypropylene needs a wider band than ABS, especially for flatness.
The international standard
Komaspec notes that general tolerances on moulded plastic parts are governed by DIN ISO 20457 (it cites the 2021-06 edition). The standard defines nine tolerance groups, TG1 to TG9, indexed to nominal size. According to Komaspec, a part is placed in a group using a points score built from five factors: the material's shrinkage behaviour, mould complexity, batch size, process stability and post-moulding operations. The tolerance values themselves are in the paid standard, so ask your moulder which group they will commit to rather than guessing it. Check which edition your drawing references, as standards are revised.
What limits the tolerance
- Resin shrinkage. Fictiv says higher-shrink materials make tolerances harder to control. Komaspec gives amorphous resins at 0.4 to 0.7 % shrinkage and semi-crystalline resins at 1 to 2.5 % (one passage of the same guide says 1.5 to 2.5 %), and says the amorphous group holds tolerances better.
- Size. Fictiv notes that bigger parts shrink more in absolute terms, and that larger holes need a wider tolerance range.
- The parting line. Komaspec and Fictiv both say dimensions that cross the parting line cannot be held as closely as dimensions contained within one mould half. Fictiv also warns that core shift can make features meant to be coaxial end up offset.
- Wall uniformity. Fictiv says uneven walls cool and shrink at different rates, which raises the risk of warp.
- Process settings. Fictiv lists injection pressure, hold time, material density and mould temperature as having a significant effect on shrinkage.
- Moisture. Komaspec notes that nylon absorbs moisture and grows after moulding, so a nylon drawing should state whether a dimension is measured dry-as-moulded or conditioned.
How to tolerance a drawing
Komaspec warns against a blanket tolerance, giving the example of ±0.05 mm on every dimension: it gets quoted high or quoted with caveats, because it tells the moulder you have not decided what matters, so they must assume everything does.
- List the dimensions that affect function: mating interfaces, sealing faces and hole patterns are Komaspec's examples.
- Put a specific tolerance on those dimensions only, and note why each one is critical.
- Apply a general tolerance (an ISO 20457 group or a commercial class) to everything else.
- Where you can, keep critical dimensions within one mould half rather than across the parting line.
- If a fit is tight, compare an amorphous resin with a semi-crystalline one before you commit.
- For hygroscopic resins such as nylon, state the measurement condition (dry-as-moulded or conditioned).
- Agree with the moulder how each critical dimension will be measured, and on how many parts, before the tool is cut.
These figures are planning values from moulding suppliers and design guides, not guarantees. Your toolmaker, the resin data sheet and first-article measurements decide what a specific part will hold.
Questions buyers ask
Can a moulded part hold ±0.025 mm?
Fictiv describes ±0.025 mm as typical for tighter applications such as medical parts, and its fine tables reach 0.030 mm for small features in some resins. That usually means a precision mould, a narrow process window and a stable resin, so expect a higher price. Ask the moulder to confirm it feature by feature.
Why did my quote come back high when I only asked for ±0.05 mm?
Komaspec's point is that a blanket ±0.05 mm on every dimension forces the moulder to treat every feature as critical. Loosening the non-functional dimensions to a general tolerance group or commercial class is often the quickest way to a cheaper quote with fewer caveats.
Should I use the SPI tables or ISO 20457?
Both are recognised ways to set general tolerances; the SPI-derived tables in Fictiv's guide use commercial and fine columns, while ISO 20457 uses tolerance groups. Pick one, name it on the drawing, and make sure the moulder quotes against the same one.
Can the tool be adjusted if dimensions come out wrong?
Often, yes, which is why first-article measurement matters. Removing steel from a cavity is generally easier than adding it back, so ask your toolmaker whether critical features will be left "steel safe" and cut to final size after trial parts are measured.
Sources
- Komaspec, Plastic part design for injection molding: https://www.komaspec.com/about-us/blog/plastic-part-design-for-injection-molding/
- Protolabs, Injection molding design guidelines: https://www.protolabs.com/services/injection-molding/plastic-injection-molding/design-guidelines/
- Fictiv, The Ultimate Guide to Injection Molding Tolerances: https://www.fictiv.com/articles/injection-molding-tolerances-an-in-depth-look