What Tolerance Can Injection Molding Hold — and How Do You Specify It on a Drawing?

Flat illustration of a molded plastic part with tolerance callouts and a caliper measuring a critical dimension.

You have finished the part design and now the drawing needs tolerances. Write numbers that are too tight and the quote comes back high. Write numbers that are too loose and the parts do not fit together.

A molded part’s tolerance comes in two parts: the tool, machined to about ±0.08 mm, and the resin, which varies by at least ±0.002 mm for every millimetre of size. Add the two together for the size you are tolerancing, and name a default class — ISO 20457 TG5 — in the title block for everything else. Tighten only the few features where fit or function actually depends on it.

How to use this guide: use the worked table to size a realistic tolerance for your part, the TG5 and SPI sections for the defaults, and the drawing checklist before the drawing goes out.

What a molded-part tolerance actually promises

A tolerance is not a promise that a dimension will be exact. It is the range of variation you accept — the amount a feature may differ from nominal and still work. Three distinctions decide how it is read on a molded part:

  • Size vs geometry. A size tolerance controls how big a feature is. A geometric tolerance — flatness, position, roundness — controls its shape and its relationship to other features. A part can pass every size tolerance and still fail to assemble if the geometry is wrong, so a flatness or position callout is sometimes worth more than a tighter size number.
  • General vs specific. A general tolerance in the title block covers every dimension that has no tolerance of its own. A specific tolerance written next to one dimension overrides the general rule for that dimension only. Most dimensions on a molded part should live on the general rule.
  • The part at measurement vs the part in service. A molded part keeps moving after it leaves the mold: it cools, it absorbs moisture, and it relaxes. Nylon, for example, takes up moisture and changes dimension with humidity. A tolerance that does not say when and under what conditions the part is measured cannot be checked fairly — a hot part and a conditioned part are not the same measurement.

A tolerance that cannot be measured is not a specification; it is a wish. Before writing any number, ask what instrument will check it — caliper, micrometer, or CMM (coordinate measuring machine) — and whether the supplier has it.

Two tolerances in one number: the tool and the resin

Injection molding has two different tolerances, and they add up. This is the first thing that makes molded parts different from machined parts, where the tolerance is mostly about the cutting tool.

The machining tolerance is the tolerance built into the mold tool itself — how accurately the steel cavity was cut. The resin tolerance is the variation in the finished molded part, caused mainly by shrinkage as the plastic cools and by normal process variation from shot to shot. Protolabs states its machining tolerance as ±0.003 in. (0.08 mm) with a resin tolerance of at least ±0.002 in./in. — that is, ±0.002 mm for every millimetre of the dimension. See Protolabs’ injection molding services.

Two points follow from those figures. First, the machining term is fixed: it is the same ±0.08 mm whether the feature is 10 mm or 200 mm across. Second, the resin term grows with size: on a 10 mm feature it is only ±0.02 mm, but on a 200 mm feature it is ±0.40 mm. That is why a large molded part cannot be held to the same tolerance as a small one, and why a drawing that asks for it will be priced accordingly.

The worked figures

The table below is an illustrative calculation using Protolabs’ published figures — machining tolerance ±0.08 mm plus resin tolerance ±0.002 mm per millimetre of nominal size. It is not a quotation, and it is not a Cavity Mold capability claim: the tolerance your part can actually hold depends on the resin grade, the geometry, the tool, and the process. The two terms are added directly here as a simplification to show scale and direction; a real tolerance analysis treats them as separate contributors.

Nominal sizeMachining toleranceResin tolerance (±0.002 mm/mm)Illustrative totalResin share of the total
10 mm±0.08 mm±0.02 mm±0.10 mm20%
25 mm±0.08 mm±0.05 mm±0.13 mm38%
50 mm±0.08 mm±0.10 mm±0.18 mm56%
100 mm±0.08 mm±0.20 mm±0.28 mm71%
200 mm±0.08 mm±0.40 mm±0.48 mm83%

Three readings. First, on small features the tool dominates: a 10 mm feature is mostly a machining question. Second, on large features the resin dominates: at 200 mm, more than four-fifths of the tolerance comes from shrinkage variation, not from the tool. Third, tightening the tool alone stops helping once the resin term takes over — a more precisely machined mold cannot fix variation that comes from the plastic itself.

Shrinkage is the reason the resin term exists, and different resins shrink by very different amounts. Protolabs’ example puts ABS shrinkage at roughly 0.003 in./in. (about 0.3%) and polypropylene at roughly 0.018 in./in. (about 1.8%) — approximate figures from its worked example. Note that the Protolabs blog prints these shrink figures with "mm/mm" labels; that is a unit slip in the blog — the figures are millimetres per inch, not per millimetre — and the same slip affects its printed resin-tolerance figure, so this article uses the US figures above instead. See Protolabs’ guide to injection moulding tolerances.

One common misunderstanding is worth clearing up: shrinkage itself is not the tolerance. The mold is cut larger than the part by the expected shrinkage, so a resin that shrinks 1.8% still produces a part at nominal size — if the shrinkage is predicted correctly. The tolerance is about the variation around that compensated size: lot-to-lot resin differences, temperature drift, and packing differences that move the actual shrinkage away from the prediction. That is why the resin grade matters so much to the tolerance, and why changing grade after the tool is cut is a dimensional decision, not just a purchasing one. Our material selection guide explains how to choose a grade and how shrinkage should be checked before the grade is frozen.

The ISO 20457 TG5 default: what it covers

If every dimension on a drawing carried its own tolerance, the drawing would be unreadable. The practical answer is a default class in the title block, and for molded plastic parts that default comes from ISO 20457, the standard for geometrical and dimensional tolerances for plastics moulded parts. Hubs / Protolabs Network states that, unless otherwise specified and agreed, any untoleranced dimension follows the TG5 class tolerances of ISO 20457. See Hubs’ guide to injection molding tolerances and dimensional accuracy.

A few things to know about that default:

  • TG5 is a general class, not a single number. The tolerance it allows grows with the nominal size of the feature — the same principle as the worked table above. The standard’s table is published as an image on the Hubs page, so this article does not reproduce its numbers; confirm the class and the values for your size range with your supplier at quote, and read them from the standard or the supplier’s published defaults.
  • Mold-related and non-mold-related dimensions are treated differently. Hubs explains the code letters: B refers to mold-related dimensions, those in the same part of the mold; A refers to non-mold-related dimensions, determined by the interaction of movable mold elements — for example wall thickness or bottom thickness, or any dimension set by shims or mold slides. A wall thickness set by two moving halves is harder to hold than a length cut into a single block of steel, and the standard reflects that.
  • The default is a starting point, not a capability claim. TG5 is what applies when nothing else is agreed. Your supplier’s actual default may differ, and the class should be confirmed in writing at quote — a default the supplier never agreed to is not a specification.

The SPI values for shape and surface marks

Size is only part of the story. For shape and for the marks the molding process leaves behind, Hubs cites the SPI Standards & Practices of Plastic Moulders for these standard values:

CharacteristicStandard value
Concentricity±0.125 mm
Roundness±0.175 mm
Flatness, dimensions up to 100 mm±0.400 mm
Flatness, dimensions above 100 mm±0.800 mm
FlashNot to exceed 0.125 mm in any direction
Ejector marksNot to exceed 0.125 mm
Gate and runner removal (protrusion or divot)±0.125 mm

These are the numbers to keep in mind when a drawing needs a flatness callout on a large cover, or when a buyer and a supplier disagree about whether a gate witness is acceptable: the limit should be written down with its cosmetic zone before the first trial, not argued over a sample.

Do not copy ISO 2768-m onto a molded-part drawing

This is the most common tolerance mistake on molded-part drawings, and it comes from a good habit applied to the wrong process. ISO 2768-1 is the general-tolerance standard for machined parts: its defaults assume material removed by cutting, where the tolerance is set by the machine tool and the fixture. A molded part is not cut; it is formed by shrinkage, packing, and cooling, and its tolerance is set by the two-part logic above. Copying "ISO 2768-m" into the title block of a molded-part drawing gives the supplier a standard the process was never built to, and gives the inspector a pass-or-fail rule that does not match how the part was made.

The consequences are practical, not theoretical. A supplier who quotes against ISO 2768-m will price the risk of a standard it cannot meet, or quietly price a secondary operation that was never discussed. A part that functions perfectly can be rejected at incoming inspection because a dimension the standard holds to ±0.2 mm was measured at ±0.3 mm — a result the molding process would have predicted and the TG5 default would have accepted. And a dispute about a rejected batch becomes a dispute about which standard the drawing meant, which is the most expensive kind of argument to have after parts have shipped.

Use ISO 20457 TG5 as the default for molded features, and reserve ISO 2768 for features that are actually machined. Many molded parts have both: a housing that is molded, with a bore that is machined afterwards for a bearing or a seal. On that drawing, the molded dimensions sit on the TG5 default and the machined bore carries its own ISO 2768 callout — and the drawing should say which is which. Our guide to tolerances on CNC machined parts explains the ISO 2768 classes and when each one applies, for the machined side of the same part.

What drives the result — and what to change first

A tolerance number on a drawing does not hold a dimension; the design, the material, and the process do. When a part will not hold its tolerance, these are the levers, in the order to try them:

  • Uniform wall thickness. Thick sections cool slower than thin ones, shrink more, and pull the surface inward — sink marks on the outside, warpage across the part. Consistent wall thickness is the single biggest contributor to dimensional stability, and it is a design decision, not a process fix.
  • Draft. Molded parts need draft — a slight taper — so they can be ejected without dragging. As a rule of thumb, 1–2° of draft works in most situations, and changing draft changes dimensions, so draft should be settled before tolerances are written, not after.
  • Gate position. Where the melt enters decides flow length, weld-line position, and how evenly the cavity packs. A weld line across a sealing face or a gate in a cosmetic zone is a design problem that no tolerance can fix.
  • Resin grade. A high-shrinkage, moisture-sensitive grade in a tight-tolerance part is a dimensional risk from the start. A filled grade shrinks less but shrinks differently along and across the flow direction, which adds warpage. Check shrinkage, conditioning, and filler behaviour against the tolerance before the grade is frozen.
  • Process control. Protolabs describes scientific moulding as optimising three parts of the process — fill, pack, and hold — so that dimensions stay consistent from run to run. Our injection molding process guide shows the process window behind that claim: melt and mold temperature, injection speed and pressure, packing pressure and time, and cooling time, each recorded with its set value, measured value, and part result. A tolerance claim that cannot point to a recorded process window is a hope, not a commitment.
  • Measurement conditions. State when the part is measured — after cooling, after conditioning, at a stated temperature and humidity — and with what instrument. A part measured hot, straight out of the mold, will read differently from the same part measured a day later, and neither reading is wrong; they are different measurements.

If the drawing is not yet final, send what you have and say so — the tolerance discussion is cheaper before the mold is cut than after it.

When to tighten — and what to do instead

Tighten only where fit, function, sealing, or alignment actually depends on it. Everything else stays on the TG5 default. When a feature does need more, the fix is often not a smaller number:

FeatureWhat drives itWhat to do instead of tightening the number
Sealing faces and boresSize plus flatness; a bore can be round and in tolerance yet still leakTighten size and add a flatness callout; check with a CMM, not a caliper
Press, slip, or interference fitsBoth mating parts, and the fit class between themSpecify the fit on both parts and gauge it; a tight number on one side alone proves nothing
Alignment-critical featuresPosition relative to a datum, not the size of each holeUse GD&T position or perpendicularity against a stated datum instead of tightening every diameter
Bearing seats and shaftsRoundness and diameter togetherAdd roundness or cylindricity; confirm the measurement method at quote
Large flat covers and panelsWarpage from uneven cooling, not tool accuracyAdd a flatness callout and fix cooling, ribs, and wall uniformity; a tighter size tolerance will not flatten a warped panel
Cosmetic surfacesGate witness, ejector marks, weld linesSpecify the cosmetic zone and the mark limits from the SPI values above, not a size tolerance
General dimensionsNothing function-criticalLeave on the TG5 default — tightening them buys inspection cost, not performance

The common mistake is to tighten every dimension instead of the one that matters. A housing with twenty dimensions at ±0.05 mm costs far more than the same housing with one sealing bore at ±0.05 mm and the rest on the default — and the two housings assemble identically.

What to write on the drawing

Before the drawing goes out, run through these checks:

  1. Default class in the title block — "General tolerances ISO 20457 TG5" so every unmarked dimension has a defined tolerance. Confirm the class with the supplier at quote.
  2. Critical features flagged — only the features that affect fit, function, sealing, or alignment carry specific tolerances. Protolabs recommends flagging up to five critical-to-quality (CTQ) features in the CAD model — a red circle on each one before the file is submitted — so the supplier’s attention goes where it matters.
  3. Datums stated — every geometric callout references a datum, so the supplier and the inspector measure from the same origin.
  4. Resin grade named — the exact grade and supplier, because shrinkage and conditioning behaviour belong to a grade, not a resin family.
  5. Measurement conditions stated — when dimensions are taken (for example, after cooling or conditioning), at what temperature and humidity, and with which instrument.
  6. Inspection method and sample size agreed — which instrument checks each tight dimension, which cavities are measured, and what evidence the first trial must supply. Our T1 sample and first-article approval guide explains the evidence package to require before production is released.
  7. Finish stated as before or after — whether each tolerance applies before or after texture, coating, or any secondary finish, especially on fit-critical features.
  8. Surface-mark limits written down — flash, ejector-mark, and gate-witness limits with their cosmetic zones, using the SPI values above as the starting point.
  9. Revision and part identity — the drawing revision on every page, so a measurement can always be traced to the definition it was checked against.

A drawing that passes all nine can be quoted without a round of clarification questions — and the price that comes back is priced against the tolerances you actually need.

Frequently asked questions

Can a molded part hold ±0.01 mm?
Not as a general tolerance: the tool alone is machined to about ±0.08 mm, and the resin term adds to that. A very small feature in a stable resin, in a controlled process, can sometimes do better — but only on that specific feature, and only when the supplier confirms it at quote with a stated measurement method. Never assume it, and never write it as a general default.

What tolerance applies if the drawing says nothing?
Whatever the buyer and the supplier agree — which is why the default should be written down before the quote, not discovered at inspection. Hubs applies the ISO 20457 TG5 class as its default for untoleranced dimensions; your supplier may use a different default, so confirm it in writing.

Should parts be measured straight out of the mold?
No, not for acceptance. Measure after the part has cooled and, where the grade requires it, after conditioning — and record when and under what conditions the measurement was taken. A result without its conditions cannot be compared with another result.

Send the drawing with the tolerance decisions already made

The fastest way to a comparable quote is to send the drawing with the tolerance decisions already on it: the ISO 20457 TG5 default in the title block, the critical features flagged, and the measurement conditions stated. Use our contact page and include the STEP file, the 2D drawing with the default class in the title block and the CTQ features flagged, the resin grade, the quantities, the key tolerances, the surface finish, and your target timing — and we will quote against those tolerances rather than assuming them. The contact form takes the initial requirements; CAD files go by email after the first reply, as the contact page explains.

Hey! I’m Jerry — a hands-on mold & CNC guy who’s spent years turning ideas into real, tangible products. From tight-tolerance molds to complex machining projects, I’ve seen (and solved) a bit of everything.

Beyond the tools and machines, I’m all about people: building trust, making things easier for clients, and finding smart solutions that work. I’ve worked with teams around the world, and I’m always excited to meet others who love creating and building as much as I do.

If you’re into manufacturing, product development, or just like a good behind-the-scenes look at how things get made — let’s connect!

Send Us Your Requirements

Let's review your mold project

Tell us what you’re building and we’ll help identify the right tooling path. Send your 2D drawing, 3D CAD file, resin, annual volume, tolerances, or target timeline when available.

Engineering-led reviewReply within one business dayConfidential project details

No obligation. We’ll review the information and reply with a practical next step. Prefer email? jerry@cavitymold.com.