Injection Molding Tolerances — Standard Grades & DFM Guide

What a molding tolerance actually is

A tolerance on an injection molded part is a contract with physics. The resin shrinks as it cools, the mold expands with heat, the machine cycles pressure up and down — and the finished dimension is the net result of all of it. Calling a tolerance does not make the process hold it; the process holds what the material, mold design and machine can deliver, and the tolerance is where buyer and supplier agree on the risk.

Most buyers over-tolerance the print. They stamp ±0.05 mm on every feature because it costs nothing in CAD — then pay 10–30% more per part, wait longer for mold trials, and fight every PPAP because a cosmetic rib is held to a sealing-feature standard. The right way is the reverse: put loose general tolerances on the drawing, and tighten only the two or three features that actually locate, seal or assemble.

This guide gives the numbers buyers can hold suppliers to: standard grades, per-material shrink, what changes with part size, and the design rules that decide whether a tight callout ships or scrapes.

Table of Contents

1. What a molding tolerance actually is
2. The Snapshot
3. Standard tolerance grades: DIN 16901 and ISO 20457
4. Tolerance by material: the shrink table
5. Tolerance by part size: bigger parts drift more
6. The 25 mm rule: dimension-dependent tolerance bands
7. Three root causes of tolerance failure
8. Wall thickness, warpage and shrink compensation
9. Mold-side factors: parting line, ejector pins, gating
10. GD&T on molded parts: call out what matters
11. DFM rules that make tolerances hold
12. How we hold tolerances: from steel to CMM
13. Measuring tolerances: first article, SPC and CMM
14. How to annotate tolerances on a drawing
15. Talking tolerances with your supplier
16. Frequently Asked Questions
17. Sources

---

The Snapshot

• Standard commercial tolerance: ±0.1–0.2 mm on general dimensions at production volume; ±0.05 mm achievable on critical features with steel-safe tooling and process control.
• Mold steel tolerance: ±0.02 mm on machined features; the mold is not the limit — resin shrinkage is.
• Amorphous resins (ABS, PC, PMMA, PS) shrink 0.4–0.7% and hold tighter tolerances than semi-crystalline resins.
• Semi-crystalline resins (PP, PE, POM, PA) shrink 1.0–3.0% and need more draft, more cooling time and wider tolerance bands.
• Standards buyers actually cite: DIN 16901 (fine/medium/coarse), ISO 20457, ISO 2768-m and, for GD&T, ASME Y14.5 / ISO 1101.
• Tolerance failures trace to three root causes: shrink variation, warpage from non-uniform walls, and parting-line/geometry limits — not “the machine.”

Standard tolerance grades: DIN 16901 and ISO 20457

The most-cited standard in injection molding sourcing is DIN 16901, which defines tolerance classes by nominal dimension. ISO 20457 is the newer international equivalent, and ISO 2768-m is the general-tolerance default many drawings inherit. Buyers rarely need to read the full standard — they need to know which grade they are paying for.

Grade	Typical use	Achievable linear tolerance	Cost impact vs standard
Fine	Critical sealing/locating features, tight assembly	±0.05 mm (small parts) to ±0.10 mm (large)	+15–30%
Medium (standard)	General functional dimensions	±0.1–0.2 mm	Baseline
Coarse	Cosmetic, non-functional, large parts	±0.3–0.5 mm	−10–20%

The practical translation most molders use: ±0.1 mm is the workhorse band for production parts up to ~100 mm. ±0.05 mm is reserved for the few features that truly need it. Beyond ±0.05 mm, you are no longer buying molding — you are buying post-machining or secondary processes, and the price reflects it.

Tolerance by material: the shrink table

Shrinkage is the dominant tolerance driver. The rule of thumb: amorphous resins shrink less and hold tighter tolerances; semi-crystalline resins shrink more and need more draft and wider bands.

Resin	Mold shrink (%)	Typical achievable (general)	Notes
ABS	0.4–0.7	±0.10–0.15 mm	Workhorse; tightest practical band
PC (Polycarbonate)	0.5–0.7	±0.10 mm	Amorphous, stable, needs drying
PMMA (Acrylic)	0.2–0.6	±0.10 mm	Optics; low shrink, brittle
PS (Polystyrene)	0.4–0.7	±0.10–0.15 mm	Amorphous, easy fill
PA (Nylon)	1.0–2.0	±0.20–0.30 mm	Hydroscopic; moisture shifts dimensions
POM (Acetal)	1.8–3.0	±0.20–0.30 mm	Semi-crystalline; tight wear parts need post-machining
PP (Polypropylene)	1.0–2.5	±0.25–0.40 mm	High shrink; living hinges
PE (Polyethylene)	1.5–3.0	±0.30–0.50 mm	Highest shrink in the commodity range
PEEK	1.1–1.4	±0.15–0.25 mm	High-temp; tight on machined features
TPU	0.8–1.8	±0.20–0.30 mm	Elastomer; dimensionally soft
PPS	0.2–0.6	±0.10 mm	Low shrink; high heat
PVC	0.2–0.5	±0.10–0.15 mm	Amorphous; low shrink

Two caveats that change the table in practice:

• Shrink is not a single number — it varies with wall thickness, fill direction and gate location. The table gives the band; the mold designer balances the part.
• Glass-filled grades shrink less in the flow direction and differently across it (e.g., 30% glass-filled PA6 drops to ~0.3–0.5% along flow but can warp across flow). Anisotropic shrink is why flat, glass-filled parts are hard to hold flat.

Tolerance by part size: bigger parts drift more

Tolerance scales with dimension, and not linearly. The same ±0.05 mm that is routine on a 20 mm feature is expensive on a 200 mm one, because shrink variation accumulates with length.

Nominal dimension	Typical commercial	Tight (with process control)
< 50 mm	±0.10 mm	±0.05 mm
50–100 mm	±0.15 mm	±0.08 mm
100–200 mm	±0.20 mm	±0.10 mm
200–400 mm	±0.30 mm	±0.15 mm
> 400 mm	±0.50 mm	±0.25 mm

These are practical bands for a well-designed, steel-safe tool at production volume. They assume uniform walls, balanced gating and a controlled process — which is what a supplier’s DFM pass is for.

The 25 mm rule: dimension-dependent tolerance bands

Buyers and suppliers need a quick way to translate nominal size into an honest band, and the industry shorthand is the 25 mm increment rule: for every additional 25 mm of nominal dimension, add roughly ±0.05 mm to the commercial band and ±0.02–0.03 mm to the tight band. This mirrors the structure of DIN 16901 and ISO 20457, which grade tolerances by nominal-size ranges rather than by a single blanket number.

Nominal dimension (mm)	Commercial (general)	Tight (critical, process-controlled)
0–25	±0.10 mm	±0.05 mm
25–50	±0.15 mm	±0.06 mm
50–75	±0.20 mm	±0.08 mm
75–100	±0.25 mm	±0.10 mm
100–125	±0.30 mm	±0.12 mm
125–150	±0.35 mm	±0.15 mm
150–200	±0.40 mm	±0.18 mm
200–300	±0.50 mm	±0.25 mm

How to use this table in practice:

• Read your critical dimensions against their nominal size, not against the general note. A ±0.05 mm callout on a 120 mm dimension is a precision program; the same callout on a 15 mm boss is routine.
• Group tight callouts on small features. Locating bosses, dowel pads and insert pockets are typically 10–30 mm — exactly where ±0.05 mm is achievable. Large envelope dimensions get the commercial band.
• When a tight callout must land on a large dimension, expect process control as a line item. It means per-shot monitoring, longer trials and possibly steel adjustment rounds — Protolabs’ published tolerance guidance makes the same point that tight tolerances require careful process control and should be reserved for critical features (https://www.protolabs.com/resources/blog/understanding-injection-molding-tolerances/).
• Cross-check against what commercial suppliers publish. FirstMold, for example, publishes a standard tolerance of ±0.127 mm for automotive programs (https://firstmold.com/industries/automotive/) — squarely in the commercial band of this table for parts up to ~75 mm. Xometry’s injection molding tolerance guidance similarly frames ±0.1 mm as the working standard with tighter bands available on critical features (https://www.xometry.com/resources/injection-molding/injection-molding-tolerances/).

Three root causes of tolerance failure

When a part measures out of spec, the cause is almost never “the machine.” It is one of three things:

1. Shrink variation — the resin cools differently across the part. Thick sections shrink more than thin ones, corners pack differently than flat walls, and the molded dimension is the average of a temperature history. Fix: uniform walls, balanced gating, controlled cycle, and shrink compensation in the steel.
2. Warpage from non-uniform walls or orientation — a rib junction or an abrupt wall change creates differential cooling, and the part bows. Fix: wall transitions, rib-to-wall ratio ≤ 0.6, and glass-filled materials designed around their flow direction.
3. Parting line, draft and geometry limits — dimensions that cross the parting line carry flash and mismatch; deep features without draft stick; and every feature needs enough draft to eject without scoring. Fix: keep critical dimensions on one side of the parting line, add draft, and move critical tolerances to features that do not cross the split.

A fourth, quieter cause is moisture: hygroscopic resins (PA, PET, TPU) absorb water, and a poorly dried lot changes dimensions part-to-part. This is why drying specs are non-negotiable for tight-tolerance nylon parts.

Wall thickness, warpage and shrink compensation

Wall thickness is the single most powerful tolerance lever a designer owns, because it controls how the part cools — and cooling is where dimensions are made or broken.

What wall variation does. A part with walls that vary more than ~2:1 cools unevenly: thick sections stay hot and keep shrinking long after thin sections have frozen. The result is sink marks over thick junctions, internal voids, and warpage as the frozen skin is pulled by the still-shrinking core. Every one of these is a tolerance failure before the part is even measured flat.

The fix list, in order of leverage:

1. Target uniform walls (1.5–3.0 mm for engineering resins). Where the design requires a thick section, hollow it with ribs instead of filling it with plastic. Ribs at 0.6–1.0× wall thickness stiffen without creating sink-prone mass.
2. Transition walls gradually. A step from 2 mm to 4 mm should ramp over several millimeters, not change abruptly. Abrupt changes create weld lines, flow hesitation and differential shrink.
3. Compensate shrink in the steel, not the process. The mold designer multiplies every cavity dimension by (1 + shrink rate) — e.g., 2.02 mm of steel for a 2.00 mm nominal in a 1% shrink resin — and then the tool is cut slightly loose on critical features (steel-safe) so it can be adjusted in after trial. This is how ±0.05 mm gets delivered in production: the steel is pre-corrected for the average shrink, and the process is tuned to hold the residual.
4. Balance gating and cooling around critical features. Gates near tight features pack them first; cooling channels sized and placed to pull heat uniformly keep the cavity temperature stable cycle to cycle. A stable die temperature is a prerequisite for a stable dimension.
5. Design against warpage, not through it. Flat, glass-filled parts warp across the flow direction; long ribs and bosses bend toward the cooling side. If the part must stay flat, add symmetric geometry or a crown in the steel that the warp flattens out.

The honest expectation: a well-designed part holds its band in production; a poorly designed part cannot be saved by a good mold or a good machine. Shrink compensation in the steel recovers the average; only uniform cooling recovers the variation.

Mold-side factors: parting line, ejector pins, gating

Even with perfect resin and a stable machine, the mold itself imposes tolerance limits. A buyer who understands these three can stop tolerance arguments before they start:

Parting line. The two mold halves meet along the parting line, and every dimension that crosses it carries two extra error sources: flash (resin that squeezes into the split, typically 0.02–0.08 mm of material you did not draw) and mismatch (the halves aligning imperfectly, ±0.05 mm or worse on large tools). Rules: put critical and cosmetic features entirely on one half; keep sealing faces and locating surfaces off the split; and know that the flash will be on the ejector side in the direction of the mold’s opening.

Ejector pins. Pins push the part off the core and leave witness marks — small circles or dimples on the ejector side. Pins also nudge the part elastically as they push, so dimensions near ejectors can see local strain and marks. Rules: keep tight-tolerance features off the ejector side where possible; put ejector marks on non-cosmetic surfaces; and expect ejector pin witness marks on every production part, no matter how clean the quote sounds.

Gating. The gate is where resin enters the cavity, and it leaves a vestige — a nub or scar that must be trimmed or machined on cosmetic faces. Gate location also decides packing: resin packs the region near the gate longest and hardest, so tight features placed near the gate hold tighter. Rules: put the gate near critical dimensions; put gates on non-cosmetic faces; and treat the gate vestige as a design feature, not a defect.

Slides, cores and inserts. Features perpendicular to the opening direction require side actions, which add cost, cycle time and their own tolerance stack (the slide-to-core interface is a second parting line). Inserts (metal or plastic, molded in) shift with their own tolerances. Every undercut you remove from the design removes a tolerance risk.

The operational rule for the whole mold side: tolerance lives in the fixed half, not the moving half. Features machined into the fixed (cavity) half are the most repeatable in the tool; features built on moving slides or across the parting line are the least. When you are deciding which dimensions deserve ±0.05 mm, choose the ones on the fixed half.

GD&T on molded parts: call out what matters

Molded prints inherit the same GD&T language as machined parts, but three callouts matter most in molding:

• Flatness — warpage control; the feature most likely to fail on glass-filled or large parts.
• Position — true position of locating bosses, inserts and mounting holes; the mold holds these via core pins, so position is repeatable when the steel is right.
• Profile / perpendicularity — mating surfaces and sealing faces; keep these on one mold half where possible.

The discipline that saves money: mark only the locating/sealing features as critical (typically 2–4 callouts on a part), put a general ±0.1–0.2 mm note on the rest, and let the supplier DFM the rest. Over-tolerancing every feature is the most expensive way to buy nothing.

DFM rules that make tolerances hold

Tolerance is designed in, not measured in. The rules that separate a part that holds ±0.05 mm from one that fights it:

• Uniform wall thickness — target 1.5–3.0 mm for engineering resins; variation of more than 2:1 invites sink and warp.
• Draft angles — 0.5–1° on walls, 1–2° on deep cores; textured surfaces need 1–3° extra per texture depth.
• Rib-to-wall ratio ≤ 0.6 — ribs stiffen without creating thick, sink-prone junctions.
• Radii at all internal corners — ≥ 0.5× wall; sharp internal corners are stress risers and flow traps.
• Critical dimensions off the parting line — a dimension that straddles the split carries ±0.1 mm of flash mismatch on top of shrink.
• Gates near critical features — filling before the feature packs it first and holds it tighter; a gate far from a tight boss leaves it under-packed.
• Drying before molding — hygroscopic resins must hit moisture spec before the shot, or every dimension drifts.

How we hold tolerances: from steel to CMM

Tolerance control is a chain, and each link is verifiable:

• Mold steel: features machined to ±0.02 mm, with shrink compensation applied in the CAD before cutting steel.
• Process control: monitored melt and mold temperature, consistent cycle time, and packing pressure tuned per shot.
• First-article inspection: CMM (coordinate measuring machine) full report on the first sample, with key characteristics mapped to the drawing callouts.
• In-process sampling: dimensional checks at defined intervals per lot, tied to Cpk where the customer’s PPAP requires it (Cpk ≥ 1.33 typical for critical features).
• Steel-safe tooling: tight features cut slightly loose and adjusted in after trial — the standard way to buy back tolerance without rebuilding the mold.

This is the same chain our DFM checklist walks through before a mold is cut, and it is why a well-DFM’d part ships within its band instead of fighting for it.

Measuring tolerances: first article, SPC and CMM

A tolerance that is not measured is a rumor. The measurement system is where tolerance arguments are actually won — and where buyers can hold suppliers to something verifiable.

First-article inspection (FAI). The first approved samples get a full dimensional report: every critical and general dimension measured, mapped to the drawing callouts, with the measurement method recorded. For molded parts the FAI is done on a CMM (coordinate measuring machine) with a probing strategy that follows the drawing datums — never a free-form scan that hides how the part actually locates. The FAI report is the contract baseline: production parts are compared to it, not to the CAD file.

SPC (statistical process control). In production, the supplier samples at defined intervals (every N cycles or per lot) and plots the critical dimensions on control charts. Two numbers matter to the buyer:

• Cpk (process capability index) — how centered and tight the process is relative to the tolerance band. Industry convention: Cpk ≥ 1.33 for critical characteristics, ≥ 1.67 for safety-critical ones. A Cpk of 1.0 means the process is exactly at the edge of the band; 1.33 means ~99.99% of parts sit inside it statistically.
• Trend, not just value — a dimension drifting toward the limit is a process problem forming, even while every measured part is still in spec. Ask for the control chart, not just the pass/fail.

Measurement discipline that prevents false arguments:

• Temperature conditioning. Plastic parts are measured at ~23 °C / 50% RH after the part has stabilized — a part straight off the press is still shrinking and will read differently than the same part 24 hours later. Nylon parts in particular must be measured in a defined moisture state (typically dry-as-molded or conditioned per the drawing).
• GR&R (gauge repeatability & reproducibility). The measurement system itself must be qualified: the same operator measuring the same part twice should get the same answer, and different operators should agree. If GR&R eats more than ~10% of the tolerance band, the gauge — not the part — is the problem.
• Same fixture, same datum. Dimensions must be measured from the drawing datums with a defined fixture. Hand-measuring from a different edge than the drawing’s datum gives a different answer every time.

The practical buyer’s rule: require the FAI report at first article, Cpk data on critical features at PPAP, and control charts on request during production. Suppliers who cannot produce these are not holding tolerances — they are hoping.

How to annotate tolerances on a drawing

Most tolerance disputes start at the drawing, because most drawings say both too little and too much. A molded-part print that suppliers can actually build to has four parts:

1. A general tolerance note. One line that says what applies when nothing is called out, e.g., “Un-toleranced linear dimensions: ±0.1 mm (ISO 2768-m equivalent); angular: ±0.5°.” This note is the default for everything, and it should be loose — ±0.1 to ±0.2 mm — because the general note is where over-tolerancing waste hides. ISO 2768-m is the common default class for general tolerances and is what most drawing templates inherit (https://www.xometry.com/resources/injection-molding/injection-molding-tolerances/).

2. A short critical-dimension list. The 2–4 features that actually locate, seal or assemble get explicit callouts (e.g., “Ø12.00 +0.03/−0.02 — true position Ø0.10 A B”). Everything else lives under the general note. If your critical list is longer than ~5 items, the design is either over-constrained or under-defined — worth a DFM conversation.

3. GD&T on the right features. Flatness on mating faces, position on locating bosses and holes, perpendicularity on sealing faces — but only where the assembly requires it. Every GD&T frame on the print adds measurement cost and trial time.

4. Molding-specific notes that prevent ambiguity:

• “Dimensions apply to molded condition” (or specify conditioned state for nylon — the drawing must state whether PA parts are measured dry or conditioned, because moisture moves them 0.1–0.3%).
• “Draft to be added per supplier DFM” — draft is a geometry change the molder must make; the drawing should authorize it rather than fight it.
• “Gate location and ejector pin marks per supplier, subject to approval” — put the gate and ejector decisions in the supplier’s DFM where they belong, with your approval gate.
• “Tolerance applies at 23 °C / 50% RH” — standardizes measurement conditions.
• “Steel-safe adjustment permitted on [critical features]” — explicitly allows the molder to cut loose and adjust in on the features you care about; without this line, molders cut to nominal and burn trial rounds adjusting.

The one-line summary: tight callouts on the list, loose general note, GD&T where the assembly needs it, and molding-specific conditions written down.

Talking tolerances with your supplier

Tolerances are negotiated, not dictated — and the negotiation happens before the mold is cut, not after the parts fail. The questions that separate a good supplier conversation from a tolerance dispute:

Before quoting:

• “What shrink rate are you using for this material grade, and where did it come from?” — the answer should be a datasheet value adjusted for the part’s wall thickness, not a generic number.
• “Which of my critical callouts can you hold as-cast, and which need steel adjustment or secondary machining?” — a supplier who answers “all of them, no problem” has not read the drawing.
• “What is your steel-safe plan for the tight features?” — confirms they will cut loose and adjust in rather than cut nominal and hope.
• “What tolerance can you guarantee at T1 (first trial) vs at production?” — prototype and production are different regimes; the production commitment is the one that matters.
• “What Cpk do you target on critical features?” — ≥1.33 is the professional answer for critical dimensions.

During the program:

• Send the critical-dimension list with the RFQ, not only the full drawing — it tells the molder what you actually care about.
• Agree in writing on the measurement method (CMM, datum scheme, conditioning) before first article, so “out of tolerance” means the same thing to both sides.
• Put the tolerance commitment on the purchase order — a verbal “we’ll hold it” is not a spec.
• When a dimension drifts out of band, ask for the control chart and the shrink/steel analysis, not a promise. The fix is usually structural (wall, gate, steel), and you need to see it.

What not to do: stamp ±0.05 mm on everything “to be safe” — it does not make parts more accurate, it makes quotes 10–30% higher and trial timelines longer. The suppliers who accept an over-toleranced print without pushback are quoting you the risk, and you will pay it later. A good molder pushes back early; that pushback is a feature, not an obstacle.

Frequently Asked Questions

1. What is the standard tolerance for injection molding? Commercial standard is ±0.1–0.2 mm on general dimensions at production volume. ±0.05 mm is achievable on critical features with steel-safe tooling and process control; anything tighter needs secondary machining.

2. What is the best injection molding tolerance? Amorphous resins like PC and ABS hold the tightest practical bands (±0.10 mm general, ±0.05 mm critical). Semi-crystalline resins like PP and POM shrink more and need wider bands unless features are post-machined.

3. What is DIN 16901? The German standard defining injection molding tolerance classes (fine/medium/coarse) by nominal dimension. It is the most-cited tolerance standard in molding RFQs; ISO 20457 is the newer international equivalent.

4. What is ISO 2768-m? A general-tolerance default class (m = medium) often inherited on drawings when no specific tolerance is called. It is a drawing standard, not a molding standard — for molded parts, DIN 16901 / ISO 20457 classes are the relevant reference.

5. Why is my part coming out out-of-tolerance? Almost always one of three causes: shrink variation from non-uniform walls, warpage from differential cooling, or dimensions crossing the parting line. Rarely the machine. A DFM pass on wall transitions and gate placement fixes most cases before steel is cut.

6. Can injection molding hold ±0.05 mm on a 200 mm part? Not commercially on a general feature. Tight tolerance scales with size: ±0.10 mm is practical to 200 mm with process control; ±0.05 mm belongs on small critical features or machined surfaces.

7. Do glass-filled materials hold tighter tolerances? Along the flow direction, yes — glass reduces shrink. But shrink becomes anisotropic (different across flow), so flat glass-filled parts can warp more. Orientation and wall design matter more than the resin’s nominal shrink.

8. How much does a tight tolerance add to cost? Going from ±0.1 mm general to ±0.05 mm on critical features typically adds 10–30% in tooling and cycle cost, plus longer mold trials. Loose general tolerances with a few tight callouts is the cheapest combination.

9. What does “steel-safe” tooling mean? The molder cuts tight-tolerance cavity features slightly loose (leaving steel to remove) instead of cutting exactly to nominal, then adjusts the steel in after the first trial based on measured shrink. It is the standard way to buy back tolerance without rebuilding the mold — and it is why the drawing should explicitly permit steel-safe adjustment on critical features.

10. Do tolerances change between prototype and production tooling? Yes, and the production commitment is the one that matters. Prototype tools (3D-printed or aluminum inserts) hold roughly ±0.15–0.25 mm and are adjusted quickly; production steel tools hold the published commercial bands and can hit ±0.05 mm on critical features after trial rounds. Never validate a tight tolerance on a prototype tool and expect it to transfer to production steel unchanged.

11. How does moisture affect nylon (PA) part dimensions? Nylon is hygroscopic: as-molded parts are dry and small, then absorb moisture from air and grow — typically 0.1–0.3% dimensional change between dry-as-molded and equilibrium-conditioned states. Tight-tolerance nylon parts must have the measurement condition written on the drawing (dry or conditioned), and the mold shrink must be set for the state the part will actually ship in.

12. What is Cpk and what value should I require? Cpk (process capability index) measures how centered and tight the process is inside the tolerance band. Industry convention: Cpk ≥ 1.33 on critical characteristics, ≥ 1.67 for safety-critical. Require the Cpk data at PPAP — a supplier who cannot produce it cannot prove the tolerance is being held statistically.

13. Can injection molding hold ±0.01 mm? Not commercially as a molded dimension — ±0.01 mm is machining territory. Molded parts go to ±0.05 mm on small critical features with steel-safe tooling; beyond that, the feature is post-machined or ground, which changes the cost structure entirely.

14. Which features should I NOT put tight tolerances on? Cosmetic ribs, large flat surfaces, dimensions that cross the parting line, ejector-side dimensions, and anything on moving slides. These inherit flash, mismatch, witness marks or slide stack-up — put ±0.05 mm only on small fixed-half features that actually locate, seal or assemble.

Sources

• Protolabs — Understanding Injection Molding Tolerances: https://www.protolabs.com/resources/blog/understanding-injection-molding-tolerances/
• Xometry — Injection Molding Tolerances (guidance and eBook): https://www.xometry.com/resources/injection-molding/injection-molding-tolerances/
• FirstMold — Automotive Injection Molding (standard tolerance ±0.127 mm): https://firstmold.com/industries/automotive/
• DIN 16901 — Tolerances for plastic molded parts (German standard, fine/medium/coarse classes by nominal dimension)
• ISO 20457 — Plastics moulded parts, tolerances and acceptance conditions (international equivalent)
• ISO 2768 — General tolerances for linear and angular dimensions (drawing default class -m)

Related resources

• DFM checklist for molded parts — wall, draft, ribs and tolerance callouts before steel is cut
• Injection molding material comparison — shrink, temperature and strength by resin
• Injection molding cost guide — what drives part price and where tolerance spend hides
• Get a quote — upload your part for a DFM review and tolerance-feasibility check