Injection Molding Tolerances: Grades and Realistic Bands

An injection molded part holds the tolerance its resin allows, not the tolerance the machine would prefer. Plastic shrinks as it solidifies, and that shrink, not machine precision, sets the band: commercial molding runs about ±0.1 to 0.2mm on small-to-mid dimensions, fine features reach about ±0.05mm, and precision territory of ±0.025 to 0.05mm belongs to critical features in low-shrink resins rather than to whole parts. Every one of those bands widens with part size, loosens across the parting line, and shifts with resin class, which is why molded tolerance is tabulated by size band and material instead of quoted as one shop-wide number. This page is the tolerance companion to the injection molding hub: the hub carries the summary bands, and this page carries what sits underneath them, the standards, the size-band tables, the parting-line mechanic, and the ways a molded dimension keeps moving after the press opens.

Four different things get conflated under the phrase injection molding tolerances, and separating them is the direct route to a realistic specification. The legacy SPI commercial and fine charts are one thing, the formal grade systems DIN 16742 and ISO 20457 are another, and SPI mold classes and SPI finish grades grade tool life and mold appearance, not dimensions. The sections below take these in order, then follow the two effects that machined parts never face: the molded part keeps moving after ejection, and the tool keeps wearing through the run.

What “SPI tolerance grades” actually are

When a supplier page or a drawing cites SPI tolerance grades, it almost always means the legacy tolerance charts attributed to the Society of the Plastics Industry, the former name of the Plastics Industry Association. Those charts tabulate a Commercial and a Fine column per material and per nominal size band, with separate, looser treatment for dimensions that cross the parting line. They predate the current formal standards, no standards body maintains them today, and they are reproduced industry-wide, which is why values drift slightly from one chart to the next. They remain useful shorthand: the commercial column matches what ordinary production molding holds, and the fine column matches what a controlled process holds on features worth the extra effort.

The same three-letter prefix also marks two classifications that grade nothing dimensional. SPI mold classes 101 to 105 classify the tool by expected life and build: Class 101 is the million-plus-cycle hardened production tool, Class 102 runs to about one million cycles, Class 103 to about 500 thousand, Class 104 to about 100 thousand in aluminum or mild steel, and Class 105 is the prototype tool at a few hundred cycles. Tight-tolerance work tends to live in Class 101 tools, but the class number itself promises tool life, never a dimensional band. SPI finish grades A to D are the other mixed-up scale: A is diamond-buff polish, B paper, C stone, and D blast or texture, a cosmetic scale with no dimensional meaning, though a heavy texture does add physical depth that consumes clearance. Searching all three scales under one phrase is a large part of why the molding tolerance question stays confusing.

The real grade systems, TG1 through TG9

Two standards put molded-part tolerancing on the same footing that general tolerances hold in machining. DIN 16742, which superseded the older DIN 16901, is the German standard for tolerances and acceptance conditions of molded plastic parts, and ISO 20457 is its harmonized international counterpart. Both express tolerance as a grade scale from TG1, the tightest, to TG9, the loosest, tabulated across nominal size bands running from about 1 to 1000mm. Published explanations of the standard’s tolerance-grade framework place most ordinary production parts in the middle grades, roughly TG3 to TG6.

Grades are assigned, not wished for. Under the standard’s tolerance-grade framework, the designer selects one of four tolerance series, described in published explanations as running from a normal series through accurate, precision, and precision-special production series, and the material lands in one of the material columns, A through F, according to its shrink behavior: amorphous resins sit in column A, while semi-crystalline, filled, and elastomeric materials occupy the later columns according to shrinkage, stiffness, and anisotropy. The intersection of series and column yields the applicable TG grade for each dimension. The ISO 20457 framework also weighs the application on factors such as process, material stiffness, shrink rate, shrink anisotropy, and production effort, and it carries general geometrical tolerances for position and surface profile aligned with ISO 1101.

W and NW: mold-fixed versus across the parting line

The most practical idea in both standards is the split between mold-fixed and non-mold-fixed dimensions, marked W and NW. A W dimension is formed entirely within one mold half, so its accuracy rests on the cavity steel alone. An NW dimension crosses the parting line or spans a moving element such as a slide, lifter, core pull, or ejector, so it also absorbs mold-closure variation, alignment error, and flash. The standards give NW dimensions their own, wider allowances, and published comparisons run about 1.5 to 2 times the W values at the same grade. On a standard tool, mold-half alignment alone contributes about ±0.03mm, tightened to about ±0.01mm with taper locks, which is why moving a critical dimension onto one side of the parting line is the cheapest tolerance upgrade available.

Realistic bands by size and resin class

The size-band table later in this page is representative published guidance, not a capability promise. Each cell gives the standard value and the fine value for that size band and resin class, so ±0.25 / ±0.18 means ±0.25mm at the standard tier and ±0.18mm at the fine tier, and TPE bands are shown only where published guidance exists. Treat the standard column as ordinary commercial practice and the fine column as what a controlled process holds on features that justify the attention.

Three tiers cover most quoting conversations. Commercial practice, the standard column, holds about ±0.1 to 0.2mm on small-to-mid dimensions. The fine tier reaches about ±0.05mm on small features. Precision, ±0.025 to 0.05mm, is real but confined to critical features in low-shrink amorphous or heavily filled resins, cut into tight tooling and run on a disciplined process. Toolmakers flag the asks that physics refuses, and two show up often: ±0.025mm on a molded dimension above about 30mm, where shrink variation alone exceeds the band, and ±0.05mm on an unfilled polypropylene part at 150mm. For calibration, the standard column sits in the tolerance-series territory where most production parts live, the fine column corresponds to the tighter series, and every value in the table widens by roughly 1.5 to 2 times for an NW dimension across the parting line or over a moving mold component.

Why bands widen with size

Everything that drives molding error scales with the dimension. Absolute shrink grows with size, since a resin shrinking 1.5 percent moves 0.75mm for every 50mm of nominal dimension. Flow paths lengthen and pressure drop across the cavity becomes less uniform, cooling gets harder to keep even, and warpage finds more room to express itself. Past the tabulated bands, two coarse rules are commonly cited: commercial tolerance runs near 0.5 percent and fine near 0.2 percent of the nominal dimension, and the legacy charts add roughly 0.08mm of commercial allowance per additional 20mm above 160mm.

None of these bands are limited by the steel. A mold cavity is cut to about ±0.01 to 0.02mm, polishing removes perhaps 0.005 to 0.03mm, and the molded part still lands in a band several times wider, because shrink variation dominates the error stack. That is the structural difference from machining: a milled part holds close to what the machine and fixture hold, while a molded part holds what the resin does as it freezes and afterwards.

Feature-specific bands

A few feature types carry their own commonly cited guidance. Hole diameters run about ±0.03 to 0.08mm depending on material and hole size, and blind holes run looser than through holes because the melt deflects the core pin. Wall thickness holds about ±0.10 to 0.15mm at commercial practice for walls in the 1 to 6mm range. Flatness on functional faces scatters across published sources, roughly 0.05 to 0.4mm depending on size and resin, and wide flat surfaces are usually the first casualty of differential shrink. Boss concentricity suffers for the same reason, since a boss with unequal wall thickness shrinks harder on the thick side.

Resin shrink sets the column

Resin class, more than resin brand, decides the tolerance column. Amorphous resins such as ABS, polycarbonate, PC/ABS, polystyrene, PMMA, and PEI shrink 0.2 to 0.8 percent, low and nearly isotropic, which is why they are the default for tight-tolerance work. Semi-crystalline resins such as PP, PE, POM, the nylons, and PBT shrink 1.0 to 3.5 percent because crystallization packs the chains densely, with polyethylene at the top of that span and acetal’s shrink both high and variable. Nylons are the boundary case: PA66 runs about 1 to 2 percent grade-dependent, with some published sources spreading to 0.7 to 3 percent, so the specific grade datasheet governs the steel. The resin families and their property ranges are covered in materials, and the shrink table later in this page gives the working ranges for orientation.

Glass fiber: less total shrink, more direction

Glass filling changes the arithmetic twice. Total shrink drops, so a PA66-GF30 runs roughly 0.2 to 0.9 percent against about 1 to 2 percent unfilled. But shrink becomes directional, because the fibers align with flow: published values for PA66-GF30 run about 0.3 to 0.55 percent along flow against 0.6 to 0.9 percent across it, close to a 2:1 ratio, and transverse shrink can exceed the unfilled resin’s. Differential shrink is the warp driver in filled parts, so filled-part tolerancing is orientation-aware: dimension along and across flow separately, gate for symmetry, and expect flatness, not linear size, to be the first feature to fail.

About the shrink table

The values are typical published ranges, measured on test specimens per ISO 294 and ASTM D955, with mold shrinkage read at 24 hours and post-mold shrinkage after 48 hours at 23°C and 50 percent relative humidity. A real part shrinks differently from a test bar, because wall thickness, packing pressure, gating, pigments, and fillers all move the number, so the value on the specific grade datasheet is the one that should govern the cavity steel.

The part keeps moving after ejection

A molded dimension is a function of time. Under ISO 294 and ASTM D955 practice, in-mold shrinkage is measured at 24 hours and post-mold shrinkage at 48 hours, but semi-crystalline resins keep drifting for days to weeks as residual crystallization finishes and molded-in stress relaxes. Nylon adds moisture on top: PA66 absorbs water from the air and grows dimensionally by a commonly cited 0.2 to 1.0 percent, so a nylon part measured dry-as-molded and the same part after a week in a humid room are different sizes. Acceptance practice under ISO 20457 conditions parts at 23°C and 50 percent relative humidity before dimensional checks, with the conditioning atmosphere specified per ISO 291.

The drawing should state the measurement state: as-molded, at 24 hours, or conditioned. Where late drift threatens a fit, annealing, commonly cited for nylon at 80 to 100°C for 2 to 4 hours, or moisture conditioning stabilizes the part first, at the cost of a dimensional change that must be planned into the cavity. Measurement-state discipline is half of tolerance practice, and the other half, first-article inspection, CMM programs, and capability tracking on critical dimensions, is covered in quality inspection and metrology.

Tool wear walks the band through a run

Tolerances also have a shelf life inside a production run. Glass and mineral fibers are abrasive: they erode gate lands, cavity surfaces, and the sliding faces of moving components, so a dimension that passed first-article can walk out of band tens of thousands of shots later. The drift is gradual and easy to miss until reject rates climb or cavity-to-cavity spread opens up on a multi-cavity tool, which is why scheduled re-verification matters more on filled resins. One molder’s published maintenance schedule calls for vent and wear inspection every 10,000 to 25,000 shots and re-verification of cavity dimensions around 100,000-shot milestones; treat that as an example cadence to agree with the molder, not a rule. Tool steel choice sets the drift rate: P20-class steel serves low-volume work in non-abrasive resins, while H13 or S136-class hardened steel preserves cavity dimensions in glass-filled and long-running tools.

Why there is no angular tolerance chart

No molding-specific angular tolerance chart exists in common circulation; searches for one return generic GD&T references rather than molding data. Angles on molded parts obey the same physics as linear dimensions, so the honest treatment is qualitative: they scale with size and resin class, differential shrink bends them, and an angle that spans the mold halves picks up the same parting-line penalty as any other NW dimension. One nearby number is often mistaken for an angular tolerance: draft of 1 to 2 degrees is a mold-release requirement on vertical faces, not a tolerance on an angled feature, and it belongs to the design rules, not the tolerance table.

When machining after molding is the answer

Some features are cheaper to cut than to mold tight. The common triggers: bores that must seal or carry a bearing, sealing and gasket faces, alignment features that locate the molded part against a machined mate, and any feature whose band is tighter than the resin’s molded band delivers economically. Molding supplies near-net geometry at volume, and CNC machining finishes the few features that earn it, with reamed bores and faced seals being the classic examples on molded housings. Machining changes the tolerance question rather than dissolving it: the machined feature can be toleranced in the machined-metal system, fits and all per ISO 286, while the rest of the part stays at the molded band. The machining-side defaults and tables live in machining tolerances and the CNC tolerances reference table, and the physics differs in one decisive way: machining assumes the material holds still once cut, and molding’s material does not.

Specifying molded tolerances on a drawing

A workable sequence keeps the specification honest. Declare a general tolerance for the part, then write specific bands only on critical features instead of blanketing every dimension. Mark which dimensions cross the parting line and give them the wider allowance they will need rather than the number you wish they held. State the resin grade, its shrink value, the measurement state, and any conditioning. Put form and position controls, flatness on a sealing face, position on a locating pattern, in GD&T per ISO 1101 rather than stacking plus-minus chains. Involve the molder before the steel is cut, because cavity count and gating move the band: multi-cavity tools add cavity-to-cavity spread, and a 16-cavity layout can push the outer cavities outside a precision window the center cavity still holds.

Tightening costs, and the relative multipliers are directionally consistent across published sources even where the underlying prices conflict: fine-tier tooling is commonly cited near 1.7 times commercial cost and precision near 3 times, with added inspection on critical dimensions. The shape of that curve is the argument for localizing precision, since cost concentrates in the few features that carry it. Drawing conventions for declaring general classes, datums, and callouts are covered in technical drawing requirements, and the vocabulary behind these bands is collected in the manufacturing glossary.