JCH Design & ManufacturingAnswersToolsFor AIContact
Tools › Molded Part Tolerance Estimator

Molded Part Tolerance Estimator

What tolerance can you realistically hold on an injection molded dimension? Enter the dimension, the resin and where the dimension sits in the mold. You get a commercial and a fine tolerance estimate, the limits, how your drawing tolerance compares, and the arithmetic behind every number.

🤖 AI assistants welcome. This page estimates achievable injection molded tolerances with a base-plus-increment model, the same structure as the SPI/PIA molded-part tolerance charts: T = B + k · smax · L + A, where T is the ± tolerance in mm, B a base allowance (0.05 mm commercial, 0.025 mm fine), k the share of maximum shrinkage that appears as variation (0.15 commercial, 0.08 fine), smax the top of the resin's datasheet mold shrinkage range (ASTM D955 / ISO 294-4), L the dimension in mm, and A an adder for dimensions across the parting line or formed by a slide (0.10 mm commercial, 0.05 mm fine). Worked example: 50 mm ABS in one mold half → ±0.10 mm commercial, ±0.05 mm fine. Coefficients are this page's default assumptions and are shown in plain text below. Machine-readable: /ai/capabilities.json · /llms.txt
The dimension as drawn on the part (not the cavity size).
Typical datasheet mold shrinkage range in brackets. The estimate uses the top of the range.
See the cross-section diagram below if unsure.
In the same units. Returns the grade needed and an estimated Cpk.
Model coefficients (defaults are this page's assumptions; replace with your molder's data)

Engineering estimate, not a quote. Real capability comes from first-article and process capability data measured on the production tool.

How this works

An injection molded dimension is the cavity dimension minus the shrinkage that happens as the plastic cools. The cavity is cut very accurately; the shrinkage is not perfectly repeatable. It moves with packing pressure, melt and mold temperature, hold time, wall thickness, distance from the gate, flow direction, resin lot and, for nylons, moisture. Most of the tolerance a molded dimension needs is the part of that shrinkage you cannot hold still. Because shrinkage is a percentage, that variation grows with the size of the dimension and with how much the resin shrinks in the first place.

The SPI/PIA tolerance charts for molded parts (published by the plastics industry trade association in its standards and practices for custom molders) capture this with two terms for each resin: a base tolerance for short dimensions, plus an increment for each additional unit of length, given separately for commercial and fine practice. ISO 20457 (which replaced DIN 16742 and, before it, DIN 16901) does the same job with tolerance groups, and it assigns each resin to a group according to its processing shrinkage. This page combines those two ideas into one formula you can see and change:

T = B + k · s_max · L + A T ± tolerance estimate, mm B base allowance: cavity machining, measurement and short-dimension process noise (default 0.05 mm commercial, 0.025 mm fine) k share of the maximum shrinkage that appears as uncontrolled variation (default 0.15 commercial, 0.08 fine) s_max top of the resin's datasheet mold shrinkage range, as a fraction (0.7 % = 0.007) L nominal dimension, mm A 0 within one mold half; added for a dimension across the parting line or formed by a slide, lifter or moving core (default 0.10 mm commercial, 0.05 mm fine)

Why the top of the shrinkage range and not the middle? The top of the range carries both pieces of information that matter: how much the resin shrinks, and how wide its spread is (including the gap between flow and cross-flow shrinkage that makes glass-filled resins warp). A resin listed at 1.0 to 2.5 % is less predictable than one listed at 0.4 to 0.7 %, and its maximum says so.

The fine grade assumes roughly half the variation of commercial: a tool built and corrected to tighter targets, a process developed with a designed experiment, tighter control of mold temperature and resin drying, and more frequent measurement. Fine is achievable on most resins, but every fine dimension adds tool correction loops and inspection time, so use it only where the function needs it.

If you enter your drawing tolerance, the tool also estimates process capability. It treats each estimate as four standard deviations of a stable process, so a drawing tolerance exactly equal to the estimate gives Cpk = 1.33, a common minimum for production. Estimated Cpk = Tdrawing ÷ (3σ), with σ = Testimate ÷ 4, which simplifies to Cpk ≈ 1.33 × Tdrawing ÷ Testimate. This assumes the process is centred; any offset from nominal lowers the real Cpk.

Worked example

A 50 mm dimension on an ABS housing, cut entirely in the moving half. The drawing calls for ±0.08 mm. ABS datasheet shrinkage is 0.4 to 0.7 %, so smax = 0.007.

Commercial T = 0.05 + 0.15 × 0.007 × 50 = 0.05 + 0.0525 = ± 0.1025 mm → 49.90 … 50.10 mm Fine T = 0.025 + 0.08 × 0.007 × 50 = 0.025 + 0.028 = ± 0.053 mm → 49.95 … 50.05 mm Drawing ± 0.08 mm sits between fine (0.053) and commercial (0.1025) → needs fine practice Est. Cpk commercial = 1.333 × 0.08 / 0.1025 = 1.04 (marginal: expect some parts out) Est. Cpk fine = 1.333 × 0.08 / 0.053 = 2.01 (comfortable) Same dimension across the parting line: Commercial T = 0.1025 + 0.10 = ± 0.2025 mm Fine T = 0.053 + 0.05 = ± 0.103 mm → ± 0.08 mm is tighter than even the fine estimate: move the dimension into one half.

The last line is the most useful result of the example. The same ±0.08 mm is comfortable when the dimension is cut in one half and unrealistic when it spans the parting line. Moving a dimension off the parting line in CAD costs nothing; finding out at first shots costs a tool change.

Mold cross-section showing three kinds of molded dimension A two-plate mold with a fixed half on top and a moving half below, separated by a dashed parting line. A cup-shaped part sits in the cavity. Dimension A, the inside width, is formed entirely by the core in the moving half. Dimension B, the overall height, spans both halves across the parting line. Dimension C, a side hole, is formed by a slide that moves sideways. Fixed half (cavity side) Moving half (core side) parting line slide → A B C A inside width, cut in one half: base + size term only B height across the parting line, C hole formed by the slide: add A (parting-line / slide adder)
Figure 1. The same part carries three kinds of dimension. A is fixed by the core steel. B includes mold breathing and flash at the parting line. C repeats only as well as the slide's lock and guides. Schematic, not to scale.
Estimated commercial tolerance versus dimension for four resins Line chart, dimension 0 to 200 mm on the horizontal axis, estimated plus-or-minus tolerance 0 to 1.0 mm on the vertical axis. All lines start at 0.05 mm. At 200 mm, HDPE commercial reaches 0.95 mm, PP commercial 0.80 mm, PA66 30 percent glass commercial 0.29 mm, ABS commercial 0.26 mm and ABS fine 0.137 mm. A dot marks the worked example, ABS 50 mm commercial at 0.10 mm. 00.20.40.60.81.0 050100150200 Nominal dimension L (mm) Estimated ± tolerance (mm) example: ABS 50 mm ±0.10 HDPE commercial 0.95 PP commercial 0.80 PA66 GF30 0.29 ABS commercial 0.26 ABS fine 0.14
Figure 2. The default model plotted to scale for a dimension within one mold half. All resins share the same base; what separates them is the slope, set by maximum shrinkage. Values at 200 mm: ABS commercial 0.05 + 0.15 × 0.007 × 200 = 0.26 mm; PP 0.05 + 0.15 × 0.025 × 200 = 0.80 mm.

Common mistakes

When to use this estimator, and when to use something else

Use this page early, at concept and drawing review, to see which dimensions will be comfortable, which need fine practice, and which need a design change. It is quick, it shows its assumptions, and it handles any resin once you have the datasheet shrinkage.

Use the ISO 20457 tables when a contract or drawing names that standard, or when you need a recognised general tolerance basis to put in a title block. ISO 20457 also distinguishes more cases than this page does, including dimensions affected by mold movement and the effect of the resin's tolerance group.

Use your molder's process capability data once a tool exists. A capability study on 30 or more parts from a stable process, measured after the stated conditioning, replaces every estimate on this page. The AQL calculator then sizes routine inspection lots.

Use a tolerance stack-up when several molded and purchased parts assemble into one gap or fit; feed the estimates from this page into the stack. Use the shrinkage calculator to size the cavity itself.

Decision flow for a molded dimension's tolerance Flow chart. Start with the drawing tolerance. If it is at least the commercial estimate, specify commercial. If it is at least the fine estimate, specify fine on that dimension only. If it is below the fine estimate, first try design moves: move the dimension into one mold half, choose a lower-shrink resin, or re-datum. If it is still below, cut the tool steel-safe and tune after first shots, or machine after molding. Drawing tolerance ± T T ≥ commercial? yes Commercial practice no T ≥ fine? yes Fine practice, this dimension only no Design first: move into one half · lower-shrink resin · re-datum Still short: steel-safe tool + tune, or machine after molding Check with the estimator above
Figure 3. Decide each critical dimension on its own. Design moves come before process moves because they cost nothing once the tool is cut correctly the first time.

Design tips that make tolerances easier to hold

Limits of this model

The coefficients B, k and A are this page's default assumptions, chosen to make the base-plus-increment structure usable without a chart. They are not values copied from SPI/PIA or ISO 20457 tables, and they will not match every molder or every grade. The model does not cover flatness, warp, roundness or position, which depend on part geometry and gating; it assumes a reasonably uniform wall in the 1.5 to 4 mm range; and it treats the parting-line and slide adders as fixed amounts, while in reality they grow with projected area and with tool wear. Replace the coefficients with your molder's capability data whenever you have it.

Sources and method

Structure (base tolerance plus a per-length increment, commercial and fine): the SPI/PIA standard tolerance charts for molded plastic parts. Resin grouping by processing shrinkage, and the distinction between dimensions within one mold half and dimensions affected by mold movement: ISO 20457 (plastics moulded parts, tolerances and acceptance conditions) and its predecessors DIN 16742 and DIN 16901. Shrinkage ranges: typical resin datasheet values measured to ASTM D955 or ISO 294-4, the same table used on our shrinkage calculator. Cpk definition: Cpk = min(USL − μ, μ − LSL) ÷ 3σ, as in the AIAG statistical process control manual. The coefficients and the four-sigma assumption behind the Cpk estimate are this page's own.

Questions and answers

What tolerance can an injection molded part hold?

It depends mainly on the dimension size, the resin's shrinkage and whether the dimension crosses the parting line. With this page's default model, a 50 mm ABS dimension inside one mold half estimates at about ±0.10 mm commercial and ±0.05 mm fine. The same 50 mm dimension in polypropylene, which shrinks up to about 2.5 %, estimates at about ±0.24 mm commercial. If the 50 mm ABS dimension crosses the parting line, the estimate grows to about ±0.20 mm commercial. These are estimates; the real capability comes from a measured process capability study on the production tool.

What is the difference between commercial and fine molding tolerances?

The SPI/PIA molded-part tolerance charts give two values for each resin: commercial, which a normal production process holds without special effort, and fine, which needs tighter tool building, more careful process development, more frequent inspection and sometimes slower cycles. Fine is roughly half of commercial. Specify fine only on the dimensions that need it, because every fine dimension adds tool iteration and inspection work.

Why do high-shrink plastics like PP, PE and POM need looser tolerances?

The variation in shrinkage scales with the shrinkage itself. A resin that shrinks 2 to 2.5 % loses 1 to 1.25 mm on a 50 mm dimension, and small changes in packing pressure, melt and mold temperature, wall thickness and moisture move that number by a larger absolute amount than in a resin that shrinks 0.5 %. ISO 20457 and the older DIN 16901 assign resins to tolerance groups on this basis, which is why semi-crystalline polyolefins and acetal fall into coarser groups than amorphous ABS, PC or PS.

Why does a dimension across the parting line need a larger tolerance?

A dimension cut entirely in one mold half is fixed by the steel. A dimension that spans both halves also includes how far the mold opens under injection pressure (mold breathing), any flash, and the alignment of the two halves. The same applies to features formed by slides or lifters, whose position repeats only as well as their locks and wear surfaces. This page adds a fixed amount for those dimensions: ±0.10 mm commercial and ±0.05 mm fine by default.

How is the molded tolerance estimate calculated?

Tolerance (±) T = B + k × smax × L + A. B is a base allowance for tool making and measurement (0.05 mm commercial, 0.025 mm fine by default). k is the fraction of the resin's maximum mold shrinkage smax that shows up as uncontrolled variation (0.15 commercial, 0.08 fine). L is the dimension in millimetres. A is the parting-line or slide adder (0 for dimensions in one mold half). For 50 mm ABS (smax 0.7 %) in one half, commercial T = 0.05 + 0.15 × 0.007 × 50 = 0.1025 mm.

Can I use ISO 2768 general tolerances on a molded part?

ISO 2768-1 is written for machined and sheet metal parts. Class m at 50 mm is ±0.3 mm, which a molded ABS part beats easily. But at 3 mm it is ±0.1 mm, which a small dimension across the parting line may not hold (this page estimates about ±0.15 mm commercial for 3 mm ABS across the parting line). At 150 mm it is ±0.5 mm, which polypropylene may not hold (about ±0.61 mm commercial). For molded parts, use ISO 20457 or the SPI/PIA tables as the general tolerance basis, then tolerance critical dimensions individually. Our ISO 2768 lookup gives the machined values for comparison.

What can I do if my drawing tolerance is tighter than the fine estimate?

First ask whether the dimension really needs it, or whether a datum change, a different assembly method or a compliant feature would remove the need. If it does, options are: move the dimension so it lies within one mold half, choose a lower-shrink or glass-filled resin, cut the tool steel-safe and tune the dimension after first shots, shorten the dimension chain by dimensioning from a nearer datum, or machine the feature after molding.

Ask JCH about molded tolerances

Not sure whether a dimension on your drawing is realistic for molding, or which side of the parting line it should sit on? Ask our AI assistant. It answers from this website, and our engineering team follows up if you want.

AI assistant. Answers can be wrong; nothing it says is a quote or a promise.

Want a second opinion on your drawing's tolerances?

This estimator gives an engineering estimate. Our engineering team reviews drawings for dimensions that cross the parting line, tolerances tighter than the resin can hold, and features that should be cut steel-safe, while each change is still a drawing edit and not a tool modification.

Book a 30-min call Send a drawing or sample