If you are designing a plastic part, the question is never “can injection molding hold ±0.05 mm?” — it is “which dimensions are worth holding that tight, and how do I write them down so my supplier can actually hit them?”
The short answer: standard commercial injection molding reliably holds ±0.100 mm to ±0.250 mm on general linear dimensions. Precision tooling can hold ±0.025 mm to ±0.050 mm — but only on a limited number of critical features, in a low-shrinkage resin, with a hardened tool and closed-loop process control. Everything outside those bounds is either a design problem or an inspection problem, not a molding problem.
This guide gives you the achievable numbers by feature type, the five variables that move them, and a specification method that stops over-tolerancing before it inflates your tooling budget.
The Short Answer: What Tolerance Can Injection Molding Actually Hold?
Tolerance in plastics is not a single number. It is a relationship between the dimension, the feature type, the resin, and the tool. Two holes on the same part can have completely different achievable tolerances.
Standard vs. precision at a glance
| Tolerance class | Typical capability (linear dims) | What it requires | Typical use |
|---|---|---|---|
| Standard / commercial | ±0.100 mm to ±0.250 mm | P20-class tool steel, conventional cooling, standard process window | Enclosures, brackets, cosmetic covers, handles |
| Functional interface | ±0.050 mm to ±0.100 mm | Better tool steel, balanced cooling, defined process window | Mating features, locators, fastener clearance, snap-fits |
| Precision (critical features only) | ±0.025 mm to ±0.050 mm | Hardened steel (H13/S7/420SS), conformal or optimised cooling, closed-loop control, cavity pressure sensing | Gear trains, sealing surfaces, optical mounts, microfluidic channels |
The critical qualifier is “critical features only.” Applying the precision band across an entire drawing is the single most common cause of unnecessary tooling cost. Reserve it for Critical-to-Function (CTF) dimensions and let a title-block tolerance govern everything else.
For a deeper treatment of how to trade precision against cost, see our guide on setting realistic and cost-effective tolerance limits.
Why Plastic Tolerances Are Not Metal Tolerances
If you copy a CNC machining tolerance block onto a plastic part drawing, you will get a part that is manufacturable in theory and unprofitable in practice. Our CNC machining tolerance philosophy is built around subtractive metal removal; injection molding is a thermal process with fundamentally different error sources.
Shrinkage is the dominant variable
Molten polymer is injected into a cavity that has been scaled up to compensate for volumetric shrinkage. The cavity is therefore cut to a size the final part never equals. What matters is not the nominal shrinkage value but how predictable and uniform that shrinkage is.
| Polymer family | Examples | Shrinkage | Tolerance behaviour | Main dimensional risk |
|---|---|---|---|---|
| Amorphous | ABS, PC, PC/ABS, PMMA | 0.4% – 0.8% | Low and largely isotropic — tight limits feasible | Sink over thick ribs and bosses |
| Semi-crystalline | POM, PA66, PBT, PEEK | 1.2% – 2.5% | Higher and anisotropic — standard limits preferred | Post-mold crystallisation and warpage |
| Glass-filled | PA66-GF30, PBT-GF20 | ~0.2% flow / ~0.8% transverse | Differential — direction-dependent | Weld-line stress and asymmetric shrink |
Semi-crystalline resins keep shrinking for hours after ejection as crystallisation completes. That is not a tooling defect; it is a material property that has to be designed around. Material behaviour is covered in more detail in our engineering plastics material selection guide.
Datum and geometry drift
Plastic parts also move because of thermal and hygroscopic expansion. A nylon part measured hot off the press, and the same part measured after two days at 23 °C / 50% RH, are two different parts. Any tolerance discussion that skips conditioning is incomplete — a point we return to in the verification section.
The Achievable Tolerance Matrix (By Feature Type)
Use this as a starting conversation, not as a contractual guarantee. Achievable tolerance is always specific to the combination of geometry, resin, tool and process — and your supplier should confirm the number for your part.
| Feature type | Standard | Achievable precision | Notes |
|---|---|---|---|
| Overall length / width (<100 mm) | ±0.150 mm | ±0.050 mm | Scaled by shrinkage predictability |
| Overall length / width (>300 mm) | ±0.400 mm | ±0.200 mm | Flow length and cooling gradient dominate |
| Wall thickness | ±0.100 mm | ±0.025 mm | Governed by tool steel and cavity pressure |
| Mating bore diameter | ±0.075 mm | ±0.025 mm | Requires core pin support and concentricity control |
| Depth of blind feature | ±0.150 mm | ±0.050 mm | Add stack-up across parting line |
| Hole-to-hole centre distance | ±0.100 mm | ±0.030 mm | Best when both holes are in the same block |
| Dimension across parting line | ±0.200 mm | ±0.100 mm | Add ±0.05–0.10 mm for tool closure stack-up |
| Dimension across a slide or lifter | ±0.250 mm | ±0.150 mm | Moving-mechanism wear accumulates |
| Flatness (small part) | 0.15 mm | 0.05 mm | Sensitive to gate location and packing |
| Angularity (per 25 mm) | ±0.5° | ±0.25° | Draft and shrink asymmetry interact |
Which numbers you can trust
Treat any published tolerance table as an indicative capability band. Three things will decide the real number for your part:
- The feature was dimensioned from a functionally chosen datum, not a convenient edge.
- The dimension does not span a moving mechanical interface if it can be avoided.
- The process window that produces it is repeatable, not a single best-case shot.
When ±0.025 mm is realistic and when it is not
±0.025 mm is realistic when: the resin is amorphous and low-shrinkage, the feature is small, both ends of the dimension are in the same steel block, the tool is hardened and the machine runs closed-loop with cavity pressure feedback.
±0.025 mm is not realistic when: the dimension crosses a parting line or slide, the resin is glass-filled and semi-crystalline, the part is larger than roughly a hand span, or the tolerance is applied to a cosmetic surface that no one will measure anyway.
Five Variables That Move Your Achievable Tolerance
1. Material shrinkage behaviour
Low-shrinkage amorphous resins (ABS, PC) give the tightest, most isotropic result. Glass-filled semi-crystalline resins give you stiffness but take bandwidth away from tolerance — fibre orientation makes shrinkage direction-dependent, so a dimension measured along flow and the same dimension measured across flow do not behave the same way.
2. Wall thickness uniformity
Non-uniform walls cool at different rates. Thin sections freeze while thick sections stay molten, producing differential shrinkage, sink marks and internal stress that shows up as dimensional drift. Ribs should generally be sized to 40–60% of the nominal wall to avoid this. See wall thickness best practice and our DFM design guide.
3. Tool construction and steel
A tool cut from P20 will not hold a precision band for a long production life. Hardened steels (H13, S7, 420 stainless) resist wear at the shut-offs and in core pins, which is where tight tolerances are actually won or lost. Cooling design matters just as much — uneven cooling guarantees uneven shrinkage. Where cycle time allows it, conformal cooling improves dimensional stability by shortening the thermal gradient across the part.
4. Process control and machine capability
A tolerance is only real if it is repeatable. That means a documented process window, closed-loop injection velocity and holding pressure, and — for precision work — cavity pressure transducers that let the machine react to what is happening inside the mould rather than to a timer. This is the core of advanced process control for precision molding.
5. Part size and flow length
Tolerance as a percentage of dimension is a useful sanity check. As a rule of thumb, expect achievable tolerance to sit in the range of ±0.05% to ±0.25% of the dimension, with the tighter end reserved for small, low-shrinkage features in a single steel block. A 300 mm dimension will not behave like a 30 mm dimension, no matter what the drawing says.
How to Specify Tolerances So They Can Be Held
Most tolerance failures are drawing failures. The part was made exactly to a drawing that was impossible to satisfy economically.
Rule 1 — Classify every dimension before you tolerate it
Split the drawing into three buckets and treat each one differently:
| Category | Tolerance to apply | Typical features |
|---|---|---|
| Critical-to-Function (CTF) | ±0.025 mm to ±0.050 mm, individually tolerated | Sealing surfaces, bearing journals, O-ring grooves, optical registers |
| Functional interface | ±0.100 mm, from the title block | Fastener clearance, locators, perimeter snap-fits |
| Non-critical | ±0.250 mm or wider | Drafted side walls, cosmetic radii, internal ribs, clearance areas |
If a dimension does not affect function, assembly or appearance acceptance, it does not deserve a tight tolerance.
Rule 2 — Use a title-block tolerance system, not 40 individual callouts
A single general tolerance note (for example, a linear tolerance block plus a separate angular tolerance) covers non-critical geometry and keeps the drawing readable. Add individual limits only where function demands them. This concentrates inspection effort and cost where it buys something.
Rule 3 — Reference a recognised plastic tolerance standard
For plastic parts, drawings should reference a plastic-specific tolerance system rather than a metal-machining default. ISO 20457 and DIN 16742 (Tolerance Groups TG1–TG9) both define tolerance bands by resin group, part size and mould complexity. They give you a defensible starting point instead of a number someone copied from a metal part. Confirm the applicable standard and tolerance group with your supplier before release.
Rule 4 — Datum for function, not for convenience
A dimension measured from a drafted side wall, a cosmetic surface or a flash-prone edge will never be stable. Choose datums on stable, functional geometry — a bore, a machined face, a locating feature — and be explicit about datum precedence. Most “the supplier can’t hold tolerance” disputes are actually datum disputes.
Rule 5 — Call out parting-line and moving-mechanism stack-up
Any dimension that spans the parting line, a slide, a lifter or a side-action accumulates tool closure and wear stack-up on top of the molding tolerance. Add roughly ±0.05 mm to ±0.10 mm to the base tolerance for these dimensions, and say so explicitly on the drawing. Parting line strategy is covered in our parting line design guide.
Sample drawing callout block
A workable title-block tolerance system for a plastic part often looks like this:
- Linear, CTF features (individually tolerated): ±0.05 mm unless otherwise specified
- Linear, general (title block): ±0.20 mm
- Angular: ±0.5°
- Draft: 1° minimum on smooth surfaces, 3° minimum on textured surfaces
- Across parting line / slides: add ±0.10 mm
- Datum system: A / B / C with datum A on the primary functional face
- Standard reference: ISO 20457 or DIN 16742, tolerance group to be agreed on DFM review
- Inspection: Cpk ≥ 1.33 on CTF dimensions, ≥ 1.67 on safety-critical features, parts conditioned 24–48 h at 23 °C / 50% RH
Tolerance vs. Cost: Where the Curve Breaks
Tightening a tolerance is not a linear cost increase. It is a step change in tooling, cycle time and inspection overhead.
| Tolerance on a given feature | Relative tooling cost | Relative part cost | Added quality infrastructure |
|---|---|---|---|
| ±0.250 mm | Baseline | Baseline | Batch inspection, gauges |
| ±0.150 mm | +10% – 25% | +2% – 5% | Sampling with gauges |
| ±0.100 mm | +25% – 50% | +5% – 12% | SPC on key dimensions |
| ±0.050 mm | +50% – 100% | +12% – 30% | CMM, climate-controlled inspection |
| ±0.025 mm | +100% – 200% | +30% – 60%+ | CMM + cavity pressure monitoring + full SPC |
Two practical consequences follow. First, precision is cheapest where it is scarcest: hold the tight band on two or three CTF features and let the rest of the part breathe. Second, the jump from ±0.050 mm to ±0.025 mm usually buys less assembly benefit than the same money spent improving a datum, a wall transition or a gate location. Our precision tooling cost breakdown walks through where that money actually goes.
Verifying Tolerance: Cpk, Conditioning and Metrology
A tolerance that cannot be verified is not a tolerance. Verification has three parts.
Why you must condition parts before measuring
Thermoplastics have high coefficients of thermal expansion, and hygroscopic resins such as nylon absorb moisture. Parts must be normalised before metrology sign-off — typically 24 to 48 hours at 23 °C (±2 °C) and 50% (±5%) RH. Measuring parts immediately after ejection produces false readings and false disputes. Our quality equipment and quality system pages describe how this is handled in practice, including FMEA, control plans, SPC and PPAP documentation, and IQ/OQ/PQ for medical work under ISO 13485.
What Cpk to require
Define the acceptance criterion on the drawing, not after a problem appears:
| Feature class | Minimum Cpk | Rationale |
|---|---|---|
| General / non-critical | Not required | Inspect by attribute or gauge |
| Functional interface | ≥ 1.00 | Adequate for assembly clearance |
| Critical-to-Function (CTF) | ≥ 1.33 | Standard production requirement |
| Safety-critical / regulated | ≥ 1.67 | Medical and safety-relevant features |
Also ask for a first article inspection (FAI) report on the T1 samples and a repeat capability study at the end of the process window, not just at nominal settings. Our T1 sample evaluation guide covers the acceptance sequence in detail.
Common Tolerance Failures and How to Prevent Them
| Symptom | Usual root cause | Prevention |
|---|---|---|
| Dimension drifts over a production run | Insufficient packing, cooling variation, tool wear at shut-offs | Closed-loop holding profile, documented process window, scheduled tool maintenance |
| Part measures in-tolerance cold, out-of-tolerance hot | Not conditioned before measurement | Specify conditioning on the drawing; define when parts are measured |
| Warpage on a flat part | Uneven wall, asymmetric cooling, off-centre gate | Balance the wall, review gate position, consider conformal cooling |
| Hole position varies cavity-to-cavity | Uneven cavity fill, unbalanced runner | Cavity-balance study, balanced runner design |
| Parting-line dimension out of tolerance | Tool closure stack-up ignored in the tolerance | Add ±0.05–0.10 mm allowance; specify which datum governs |
| Glass-filled part fails a transverse dimension | Fibre-orientation shrink asymmetry | Widen the limit or reorient the gate |
Many of these symptoms overlap with classic molding defects. Our common injection molding defects guide maps symptoms to root causes and process corrections.
Supplier Capability Checklist
Before you release a drawing with a precision band, confirm your supplier can answer these:
- Which tolerance standard do you work to, and which tolerance group will you assign this part?
- What is your documented capability on comparable features, with a Cpk study — not just a statement?
- Are the machines assigned to this tool closed-loop, and do you use cavity pressure sensing for precision work?
- What steel will the cavity and core be cut from, and what is the expected tool life at this tolerance?
- Do you produce a DFM review that flags tolerances that cannot be held before the tool is cut?
- How and when are parts conditioned before dimensional inspection, and on what equipment?
- What is the inspection plan for CTF dimensions — first article, then ongoing SPC frequency?
- Who signs off the process window, and what happens when a dimension trends toward the limit mid-run?
A supplier who answers these with documents rather than adjectives is a supplier who can hold a tolerance. GoodTech supports this with an engineering-driven process — DFM review and mold flow analysis before tooling release, closed-loop molding, and ISO 9001 / IATF 16949 / ISO 13485 aligned quality systems.
FAQ
What is the standard tolerance for injection molded plastic parts? General linear dimensions are typically held to ±0.100 mm to ±0.250 mm in normal production. Precision features can reach ±0.025 mm to ±0.050 mm, but only on a limited number of critical dimensions, in a low-shrinkage resin, with hardened tooling and closed-loop process control.
Can injection molding hold ±0.05 mm on every dimension? No — and a drawing that demands it will be expensive and will still generate disputes. ±0.025 to ±0.050 mm is achievable on individual CTF features. Applied across an entire part, it multiplies tooling cost, slows the cycle and forces full CMM inspection with little functional benefit.
Which tolerance standard applies to plastic parts? Plastic-specific systems are preferred over metal-machining defaults: ISO 20457 and DIN 16742 (Tolerance Groups TG1–TG9) define bands by resin group, part size and mould complexity. The applicable standard and group should be agreed with your supplier during DFM review.
How much does tightening a tolerance cost? Expect roughly +50% to +100% tooling cost and +12% to +30% part cost for moving from ±0.050 mm to ±0.025 mm, plus dedicated metrology. The increase is a step change driven by steel, cooling design, cycle time and inspection, not a smooth curve.
Why do parts measure differently a week later? Because semi-crystalline resins continue to crystallise and hygroscopic resins absorb moisture after ejection. Parts must be conditioned — typically 24 to 48 hours at 23 °C and 50% RH — before dimensional inspection. Measuring hot parts invalidates the reading.
Should I apply the same tolerance to a dimension across the parting line? No. Dimensions spanning the parting line, a slide or a lifter accumulate tool closure and wear stack-up. Add approximately ±0.05 mm to ±0.10 mm to the base tolerance, or redesign so the dimension sits within a single steel block.
What Cpk should I require? Cpk ≥ 1.33 is a reasonable production requirement for critical-to-function dimensions. Safety-critical or regulated features — for example in medical device components — commonly require Cpk ≥ 1.67, with documented SPC over the full process window.
Can 3D printing validate a tight tolerance before tooling? Only for form and fit. Additive processes do not reproduce anisotropic shrinkage, weld lines or molecular orientation, so they cannot validate a molding tolerance. Use prototype or bridge tooling and functional sampling for that. See our rapid prototyping capabilities for where prototyping does help.
Key Takeaways
- Standard injection molding holds ±0.100 mm to ±0.250 mm; precision tooling reaches ±0.025 mm to ±0.050 mm on critical features only.
- Shrinkage predictability — not the nominal shrinkage value — sets your achievable tolerance. Amorphous resins hold tighter than semi-crystalline and glass-filled resins.
- Communicate tolerance through a title-block system plus individual CTF callouts, referencing ISO 20457 or DIN 16742 rather than a metal tolerance block.
- Always add stack-up allowance for dimensions crossing the parting line or moving mechanisms.
- Require Cpk ≥ 1.33 on CTF features (≥ 1.67 on safety-critical), parts conditioned 24–48 h at 23 °C / 50% RH, and FAI reports on T1 samples.
- Spend precision where it pays: two or three CTF features, correct datums, uniform walls — not blanket tight tolerances.
Ready to check what your part can actually hold? Send us your STEP or IGES files. Our engineers return a DFM review that flags unachievable tolerances, proposes realistic limits, and prices the tooling accordingly — with NDA-backed confidentiality from the first file transfer.
