Injection Molding Tolerances: What’s Achievable and How to Spec Them
Injection Molding Tolerances: What’s Achievable and How to Spec Them
Injection molding tolerances determine whether your part fits, functions, and passes inspection, and misspecifying them is one of the most expensive mistakes in tooling. Over-tight tolerances on the wrong features routinely add $8,000 to $25,000 to mold cost and 3 to 4 weeks to build time. This guide covers achievable ranges by material, the two dominant standards (DIN 16901 and ISO 20457), and exactly how to call out plastic part tolerances on your drawings.
Why Injection Molding Dimensional Accuracy Has Hard Limits
Plastic is not metal. Every thermoplastic shrinks as it cools, and that shrinkage is never perfectly uniform. Wall thickness variation, gate location, mold temperature gradients, and packing pressure all shift where material ends up relative to where you drew it. You are not machining a block of aluminum to a fixed geometry. You are freezing a flowing fluid in a cavity, and that process has natural variation baked in.
The practical floor for general injection molding dimensional accuracy on a well-built production tool is roughly ±0.002 in. (±0.05 mm) on features under 1.0 in., using a stable semi-crystalline or amorphous resin in a properly temperature-controlled tool. Below that floor, you are in precision or micro-molding territory, and the economics change fast.
Three physical factors set the ceiling on what any molder can hold:
- Material shrinkage rate and its batch-to-batch variability (ranges from 0.1% for glass-filled nylon to 2.5% for unfilled polypropylene)
- Thermal gradients across the mold, which create differential shrinkage across a single part
- Parting line flash and ejector pin displacement, which add mechanical variation independent of material behavior
None of these go away with better machining. They are managed through tool design, process control, and material selection. If your drawing calls for ±0.001 in. on a feature that crosses the parting line in an unfilled PP part, no offshore or domestic molder can reliably hit it.
DIN 16901 and ISO 20457: The Two Standards You Need to Know
Most drawing packages in North America either use no formal tolerance standard for plastics (a serious mistake) or reference one of two international frameworks. Understanding both prevents miscommunication with your toolmaker, especially when sourcing offshore.
DIN 16901 is the older German standard, published by Deutsches Institut für Normung, and it remains the most widely referenced document for plastic part tolerances in global tooling. It defines tolerance grades from FG 1 (coarse) through FG 7 (precision) based on nominal dimension ranges. Grade FG 4 is roughly the default achievable on a production tool without special process controls. Grade FG 6 and FG 7 require controlled tool temperature, tight resin lot control, and often dedicated presses.
ISO 20457 is the current international standard for injection-molded part tolerances. Published by the International Organization for Standardization, ISO 20457 specifies a tolerance system with classes A (general purpose) through D (precision), tied to nominal dimension and material group. It maps closely to DIN 16901 in spirit but uses a cleaner material grouping system and is the preferred reference for new programs.
In our shops and on drawings we review for clients, we see DIN 16901 cited far more often on existing programs. For new tooling, we recommend ISO 20457 as the primary callout, with DIN 16901 as a secondary reference if your supply chain is accustomed to it. Either is acceptable. What is not acceptable is leaving tolerances as ±0.005 in. (all) on a plastic part drawing, which is what we see on roughly 40% of the initial drawing packages we receive.
Achievable Injection Molding Tolerances by Material
Material choice is the single biggest variable in what tolerance is achievable at a reasonable cost. Amorphous resins like ABS, PC, and PMMA shrink less and more predictably than semi-crystalline resins like nylon, acetal, and polypropylene. Glass or mineral fill tightens shrinkage considerably and is one of the fastest ways to improve dimensional stability without changing part geometry.
The table below shows typical achievable tolerances for general production tooling (SPI Class 103 equivalent) on features under 4.0 in. nominal. These are realistic production values, not best-case lab results. Data is consistent with DIN 16901 FG 4 to FG 5 and ISO 20457 Class B to C benchmarks.
| Material | Shrinkage Rate (%) | General Tolerance (±in.) | Precision Tolerance (±in.) | Notes |
|---|---|---|---|---|
| ABS (unfilled) | 0.4 to 0.7 | 0.003 | 0.001 | Good baseline for amorphous parts |
| PC (unfilled) | 0.5 to 0.7 | 0.003 | 0.001 | Tight batch control needed for precision |
| PC/ABS blend | 0.5 to 0.7 | 0.003 | 0.0015 | Slightly more variable than pure PC |
| Nylon 6/6 (unfilled) | 1.0 to 1.5 | 0.005 | 0.002 | Hygroscopic; condition before measuring |
| Nylon 6/6 (30% GF) | 0.3 to 0.6 | 0.003 | 0.001 | Anisotropic shrinkage; flow direction matters |
| Acetal (POM) | 1.8 to 2.2 | 0.005 | 0.002 | Excellent long-term stability post-shrinkage |
| Polypropylene (unfilled) | 1.5 to 2.5 | 0.007 | 0.003 | Hardest material for tight tolerances |
| PP (20% talc filled) | 0.8 to 1.2 | 0.005 | 0.002 | Much better than unfilled; common in automotive |
| PMMA (acrylic) | 0.3 to 0.5 | 0.003 | 0.001 | Brittle; optical-grade needs cosmetic controls too |
| PEEK (unfilled) | 1.1 to 1.4 | 0.004 | 0.0015 | High process temperature; stable tool required |
Precision tolerances in the right column require dedicated process setup, in-cavity sensors in many cases, and a tool built to at least SPI Class 101 or 102 with H13 or hardened P20 steel in the core and cavity. Expect a 20% to 35% premium on tool cost and 2 to 3 additional weeks of build time compared to a general-tolerance tool.
How Feature Size and Geometry Affect What You Can Hold
Tolerance bands widen as nominal dimension grows. This is baked into both DIN 16901 and ISO 20457. A ±0.002 in. tolerance on a 0.5 in. bore is achievable. The same ±0.002 in. on a 12.0 in. overall length is not, regardless of material or tool quality. Shrinkage error scales with part size, and so must your tolerance bands.
As a working rule: for every inch of nominal dimension beyond 2.0 in., open your general tolerance by 0.001 in. per inch. A 6.0 in. length in ABS that you might hold to ±0.003 in. at 1.0 in. nominal should be called out at ±0.007 in. for a production drawing. Tighter than that requires post-mold sizing or dedicated fixtures and process holds.
Feature type also matters significantly for gd&t plastic parts. Circular features (bores, bosses, pins) are more consistent than linear lengths because the mold steel controls them symmetrically from the centerline. Features that cross the parting line carry additional variation from mold alignment and wear, typically adding 0.001 in. to 0.003 in. of uncertainty on top of material shrinkage. Features formed by side actions or lifters carry similar additional variation.
Flatness and straightness on long, thin walls are especially difficult to control. A 0.100 in. wall at 4.0 in. in length will warp post-ejection in nearly every semi-crystalline material unless you add ribs, cooling fixtures, or accept a flatness callout of 0.010 in. or more.
How to Specify Plastic Part Tolerances on Your Drawings
Most tolerance problems we see come from one of three drawing errors: using a metal part tolerance block on a plastic part, calling out GD&T with no acknowledgment of the parting line, or applying uniform tight tolerances to every feature regardless of functional importance. All three inflate mold cost and create inspection failures on features that do not matter to the assembly.
The correct approach is to apply a tiered tolerance strategy:
- Functional critical dimensions (mating bores, snap-fit engagement lengths, sealing surfaces): call out with explicit tolerances per ISO 20457 Class C or tighter, flagged as Key Characteristics (KC) per your internal QMS
- Secondary functional dimensions (boss-to-boss spacing, datum hole locations, wall thicknesses): ISO 20457 Class B or DIN 16901 FG 4, called out in the general tolerance block
- Non-functional dimensions (cosmetic surface extents, fillet radii, logo boss heights): ISO 20457 Class A or DIN 16901 FG 3, called out in the general note
For your general tolerance block, replace the standard metal block with a note that reads: “Unless otherwise specified, plastic part tolerances per ISO 20457 Class B. Material shrinkage per resin supplier datasheet. Measure at 23°C / 50% RH per ISO 294-4.” That single note eliminates at least half of the post-mold inspection arguments we see on new programs.
When applying GD&T to plastic parts, use datum references that are accessible in the mold, not datums that require a mating part to establish. A datum A on the top face of a lid that is formed by a moving half of the tool will shift with every tool maintenance cycle. Anchor your datum scheme to features in the fixed half whenever possible, and clearly note which features are “as-molded” vs. “post-machined” if secondary operations apply.
One non-negotiable rule: do not carry tighter than ±0.005 in. on a parting line feature in any unfilled semi-crystalline resin. If the function demands it, redesign the part to move that feature away from the parting line, or specify a post-mold secondary operation with a separate inspection characteristic.
The Cost Impact of Over-Tightening Tolerances
Tighter tolerances cost money in four places: tool build, tool steel selection, process qualification, and ongoing inspection. A mold built to hold ±0.001 in. on critical bores requires H13 core and cavity steel instead of P20, EDM-finished cavity surfaces instead of milled and stoned, and likely a hot runner with valve gates to control fill precisely. That combination adds $12,000 to $20,000 to a mid-size tool on its own.
Process qualification for a precision-tolerance tool typically requires a full PPAP or equivalent first article with Cpk measurement on every KC dimension. On a 20-KC-dimension part, that inspection run costs $3,000 to $6,000 in CMM time alone, plus 1 to 2 weeks of calendar time before you can release the tool to production. If the mold requires a steel correction after first article, add another $4,000 to $9,000 and 2 to 3 weeks.
The math is straightforward. If you apply ±0.001 in. tolerances to 15 dimensions when only 4 of them are functionally critical, you have paid for precision on 11 features that do not need it. On a tool budgeted at $45,000, that decision can push final cost to $62,000 or more. Audit your tolerance callouts before you release the design for quote. Our project managers run this check on every new program before we request tooling quotes.
Frequently Asked Questions
What is a realistic general tolerance for an injection-molded ABS part?
For features under 2.0 in. on a production tool, ±0.003 in. is a reliable general tolerance for unfilled ABS. For features between 2.0 in. and 6.0 in., open that to ±0.005 in. to ±0.007 in. depending on geometry. These values align with DIN 16901 FG 4 and ISO 20457 Class B for the ABS material group.
Does DIN 16901 or ISO 20457 apply to my drawings?
Either standard is acceptable on a drawing; they are compatible in practice. ISO 20457 is the current preferred standard for new programs because it uses cleaner material groupings and is maintained by ISO. DIN 16901 is still widely understood by toolmakers worldwide, including in China, so referencing both in a drawing note creates no confusion and maximum clarity.
Can I hold ±0.001 in. on a parting line feature?
Rarely, and only with amorphous resins, a precision-built tool (SPI Class 101), and dedicated process controls. Even then, mold wear over the tool’s life will erode that capability. The better engineering answer is to redesign the part so that feature is not on the parting line, or accept a secondary operation to hit that tolerance reliably.
How does glass fill affect injection molding tolerances?
Glass fill reduces shrinkage rate significantly, which tightens achievable tolerances. Unfilled nylon 6/6 shrinks 1.0% to 1.5% and holds about ±0.005 in. general tolerance. At 30% glass fill, shrinkage drops to 0.3% to 0.6% and general tolerance tightens to ±0.003 in. The trade-off is anisotropic shrinkage: the part shrinks less in the flow direction than perpendicular to it, which requires careful gate placement to control warpage.
What is the right way to measure a molded plastic part for dimensional compliance?
Per ISO 294-4, measure at 23°C and 50% relative humidity after a minimum 24-hour conditioning period at those conditions. For hygroscopic materials like nylon, condition per the resin supplier’s datasheet, which may require a longer soak. CMM measurement is standard for KC dimensions; optical comparator or digital calipers are acceptable for general tolerance features if calibrated and traceable. State the measurement standard on the drawing, not just in your QMS.