Quick answer
Tight tolerances raise cost through five paths: more precise and adjustable tooling, more engineering and tool trials, a narrower process window, more capable measurement, and a higher risk of scrap or secondary work.
A requirement comfortably inside proven production capability may add little. A limit near that capability needs better centering, validation, maintenance, and inspection. A limit outside stable as-molded capability may need a redesign, a different resin or mold concept, sorting, or post-machining.
The buying rule: tighten only the features that protect fit, seal, movement, safety, or another defined function. Quote the rest under an appropriate general tolerance and compare suppliers on cost per acceptable part—not mold price alone.
Where tolerance cost appears
Why tolerance cost is nonlinear
A tolerance is the allowed variation from a stated nominal size or geometry. The drawing creates an acceptance boundary, but it does not prove that a manufacturing system can hold that boundary repeatedly. Cost depends on where the limit sits relative to actual variation.
Imagine a stable feature whose production spread fits easily inside the specification. A modestly tighter limit may require no change. As the window narrows, ordinary variation starts approaching the limits. The supplier then has to center the process more carefully, reduce variation, inspect more parts, or price rejected output. Narrow it again and the project may need another gate, a more adjustable tool, fewer cavities, a controlled material source, longer cooling, or a secondary machining step.
No credible universal multiplier exists. Statements such as “halving a tolerance doubles cost” ignore feature type, nominal size, resin grade, flow direction, gate and cooling, cavity count, process stability, inspection, volume, and supplier capability. Ask which specific requirement changes the manufacturing plan and by how much.
Start with function
Prove the requirement before cutting steel
For every tight dimension, ask what fails outside the limit. Is it a seal, snap engagement, bearing fit, connector position, filling-line interface, appearance gap, safety clearance, or regulated performance point? If the answer is unclear, the decimal places may be controlling nothing useful.
Build the full assembly stack first. Include mating components, fastener clearance, fixture location, seal compression, thermal movement, moisture, and expected deformation. Tightening one molded feature cannot rescue a stack dominated by another component.
Prototype fit, movement, force, and leakage where practical. A prototype may not reproduce production shrinkage, but it can expose a wrong datum, impossible clearance, or unnecessary requirement before tool changes become expensive.
Mold precision is not finished-part precision
A tool shop may machine cavity steel very accurately, but the plastic part still experiences pressure, flow orientation, packing, cooling, ejection, shrinkage, residual stress, post-mold relaxation, moisture exchange, and use temperature. Mold accuracy removes one source of error; it does not cancel the others. Do not accept a steel-machining tolerance as proof of molded-part capability.
Shrinkage changes size; warpage changes shape. A part can shrink predictably and stay flat, or meet an average size while bowing or twisting. A simple cavity scale factor helps with predictable size change but cannot correct every local distortion.
The current ISO 294-4:2018 method distinguishes molding and post-molding shrinkage, as well as directions parallel and normal to melt flow. It also treats humidity uptake as part of post-molding and total shrinkage rather than molding shrinkage. That makes the direction and condition important—but a test specimen value is still not a guaranteed tolerance for a production part.
Cost map
Six ways a tight tolerance changes the quote
Separate upfront from recurring cost. Better cooling or a replaceable critical insert may raise the mold investment but lower scrap later. Permanent inspection, slower cycles, sorting, restricted cavities, or machining raise every accepted part. Ask for both.
Tool strategy
Design the tool for correction and wear
Features made within one rigid mold half often have fewer mechanical contributors than dimensions spanning a parting line or moving slide. Actions need operating clearance, locking, guidance, and wear control. If related precision features can be formed together, repeatability may improve.
For uncertain critical features, consider separate inserts and an intentional correction plan. “Steel-safe” means leaving a feature so the tool can be adjusted in a planned direction after sampling. That direction depends on whether core or cavity steel forms the feature; it must be reviewed feature by feature.
The Honokage equipment page lists CNC, EDM, other moldmaking equipment, injection molding machines, and a 3D CMM. Treat these as supplier-provided capability statements and request the machine, accuracy, calibration, maintenance, and drawing-specific evidence relevant to your project.
Which molded features are expensive to control?
No feature is automatically impossible or cheap. Difficulty comes from how geometry, tool architecture, flow, cooling, material, and measurement interact. The table below is a conversation starter for DFM, not a universal capability chart.
| Requisito | Why cost rises | Lower-cost response |
|---|---|---|
| Short hole or boss | Pin, cooling, packing, draft, and ejection affect size. | Control the functional diameter; relax unrelated depth and appearance. |
| Long overall size | Shrinkage, temperature, flow direction, and setup accumulate. | Dimension from functional datums; avoid a tight envelope without need. |
| Broad-panel flatness | Uneven cooling, ribs, gates, and orientation create bow or twist. | Improve geometry and flow; control assembled profile if appropriate. |
| Across parting line | Two mold halves, alignment, clamp behavior, mismatch, and flash contribute. | Keep related precision features in one half when possible. |
| Slide or insert position | Moving clearance, loading, lockup, flow force, and wear add variation. | Add positive location, guidance, replaceable inserts, and clear datums. |
| Seal or snap function | Several dimensions and material behavior interact. | Control the critical stack and add leak, fit, force, or retention tests. |
| Multi-cavity match | Each cavity fills, cools, wears, and measures differently. | Identify and qualify every cavity; plan cavity-specific correction. |
Use GD&T to express function, not decorate a drawing
Repeated plus-minus coordinate dimensions can overconstrain a part while failing to describe how it assembles. Geometric dimensioning and tolerancing, or GD&T, can reduce cost when it creates a functional datum reference frame and uses position, profile, orientation, flatness, or runout to describe the real tolerance zone.
For example, a clearance-hole pattern may be better controlled by position relative to mounting datums than by tight independent X and Y dimensions. A mating perimeter may be better expressed by a surface profile than dozens of two-point sizes. A seal land may need local flatness plus a separate surface-defect rule and a leak test.
State one governing system and edition. ISO 1101:2017 defines ISO geometrical-tolerancing language, while ASME Y14.5-2018 (R2024) is widely used in U.S.-based product definition. Do not mix meanings casually, and agree how the inspector will establish each datum.
Stable production
A stable process window costs less than constant adjustment
A robust process makes acceptable parts across a justified operating window. A fragile process works at one narrow setting and depends on frequent operator correction. Tight dimensions supported only by continuous tweaking should be priced as recurring risk.
Injection-molding simulation can add development cost, but it may expose filling, pressure, fiber-orientation, and warpage risks before steel changes. BASF’s simulation guidance describes using those results to optimize geometry, gate location, and process parameters.
In a multi-cavity mold, keep cavity identity in samples and routine records. Pooled data can hide one poor cavity behind several good ones. Balance the runner and cooling, then review every cavity under the intended material, machine, cycle, and conditioning.
Acceptance must be measurable
Measurement can consume the tolerance budget
The reported value includes more than the part. Fixture, instrument, operator, alignment, surface, algorithm, environment, and sampling can add variation. A very tight limit paired with an unsuitable gauge creates false rejects, hidden process change, or buyer-supplier disputes rather than real precision.
ISO 14253-1:2017 addresses conformity decisions near specification limits while considering measurement uncertainty. Buyers and suppliers should agree the decision rule and dispute method before the first tool approval.
A functional gauge or test can sometimes evaluate the real risk more directly: a master mating part, a clearance-pattern gauge, leak test, snap-force curve, or fixture-based assembly check. It complements—not replaces—clear drawing and process controls.
Capability evidence
A passing first article is not process capability
A first article shows that measured samples passed at one point. Capability asks whether a stable, representative production process can continue fitting inside the limits. Cp compares tolerance width with estimated process spread; Cpk also considers centering. The result depends on the study method, stability, sampling, distribution, cavities, and measurement system.
Do not demand one universal Cpk target for every dimension. Tie the index and target to risk, then define sample size, subgrouping, machine, material lots, cavities, conditioning, measurement method, and reaction plan. Cpk from a small, unstable, pooled, or poorly measured sample can mislead.
Honokage testing page shows supplier-stated raw-material, mold-setup, injection, first-sample, and finished-inspection steps. For a project, ask for the actual control plan, calibrated method, all-cavity data, capability study definition, functional results, and records.
How to reduce tolerance cost without weakening function
Separate cosmetics. Sink, unwanted flow structures, roughness, and joint lines are explicitly outside the scope of ISO 20457:2026. Set visual zones, viewing conditions, limit samples, flash or mismatch rules, and surface requirements directly. Tightening unrelated dimensions is a costly and unclear way to control appearance.
Standards update
Use the correct standard and edition
As of August 13, 2026, ISO 20457:2026 is the current published second edition; ISO 20457:2018 is withdrawn. The new edition addresses geometrical and dimensional tolerances, manufacturing effort for direct tolerances, general tolerances, and acceptance conditions for covered plastic molding processes. It does not guarantee that every supplier, resin, geometry, and tool can achieve every tolerance.
Do not automatically put ISO 2768-1 on a new molded-plastic drawing as the manufacturing-capability basis. Its stated scope covers workpieces made by metal removal or sheet-metal forming, while ISO 2768-2 is withdrawn. Use the plastic-specific framework, applicable product standards, and explicit CTQs agreed with the molder.
Never write only “per ISO.” State standard, year or edition, applicable class or agreement, drawing rules, material assumptions, datums, conditioning, measurement method, acceptance state, and which document controls if CAD, drawing, quality plan, supplier standard, and purchase order conflict.
Tolerance-ready RFQ checklist
Send the same controlled package to every supplier so price differences reflect capability and scope rather than different assumptions.
Red flags in a tolerance quotation
Compare lifetime cost
Normalize every quote to an acceptable part
Ask whether the offer is priced per shot, per molded part, or per accepted part after inspection. Check who pays for startup scrap, cavity imbalance, gauges, first-article layouts, capability studies, sorting, tool corrections, preventive maintenance, rejected production, and requalification after a change.
A higher-precision mold may be the lowest-cost choice at high volume if it improves stable yield and avoids permanent inspection. Post-machining can be sensible when only one or two features exceed economical as-molded capability, especially at moderate volume. Include fixtures, chips, cleaning, datum transfer, cycle, and inspection in that comparison.
The useful denominator is total lifetime spending divided by acceptable output at the required performance—not the cheapest mold, fastest sample, or lowest nominal piece price.
Frequently asked questions
What is a standard injection molding tolerance?
There is no single universal value. ISO 20457:2026 provides a molded-plastic tolerance and acceptance framework, but achievable capability still depends on feature, size, resin, geometry, gate, cooling, mold, cavities, process, conditioning, and measurement.
Does every tighter tolerance increase cost?
Not necessarily. A requirement inside proven normal capability may add little. Cost rises when the limit changes the tool, material controls, trials, process window, inspection, yield, maintenance, or secondary operations.
Can injection molding hold ±0.05 mm?
Some small, well-supported features may do so under suitable conditions, but it is not an industry-wide or Honokage-wide promise. Define the exact feature, nominal size, datum, material, condition, cavities, method, volume, and capability evidence before accepting it.
What is the difference between mold and part tolerance?
Mold tolerance describes machined and assembled tooling. Part tolerance applies to the finished plastic, which also reflects shrinkage, warpage, packing, cooling, flow orientation, moisture, temperature, wear, and measurement.
Can GD&T lower molding cost?
Yes, when functional datums and tolerance zones replace ambiguous or excessive coordinate limits. It can raise cost when symbols are unclear, datums are unstable, inspection is undefined, or the geometry has no functional justification.
Does ISO 20457 guarantee capability?
No. It provides specification and acceptance concepts within its scope. The project still needs material, geometry, tooling, production, measurement, and functional validation. It also does not cover listed surface imperfections such as sink marks and joint lines.
Should every CTQ require Cpk?
No universal rule applies. Choose capability evidence by risk, then state the index, target, study method, sample size, subgroups, cavities, lots, stability, conditioning, measurement system, and reaction plan.
When should a feature be post-machined?
Consider it when only a few features need accuracy beyond stable as-molded capability, when volume is moderate, or when the final reference exists only after assembly or conditioning. Compare all recurring machining and inspection cost with a more capable mold and process.
Project review
What to send for a tolerance and cost discussion
Honokage IML Solutions page states that the supplier supports product requirements, CAD development, prototyping, in-house tooling, mold-flow work, production, and quality planning. These are supplier statements, not a drawing-specific capability guarantee.
For a useful review, send native 3D CAD, a controlled drawing, exact resin and color/additive assumptions, mating-part data, annual and lifetime volume, service temperature and humidity, the CTQ list, cosmetic zones, functional tests, target cavities, inspection conditions, and expected capability evidence.
Protect function with the fewest necessary constraints
The lowest-cost drawing is not the loosest one. It is the drawing that makes critical performance clear and gives the molder freedom everywhere else. Mark CTQs, analyze the assembly stack, choose stable functional datums, separate size from geometry and appearance, agree how and when parts are measured, and validate every production cavity.
Then compare the one-time and recurring cost of holding those requirements through the program life. The goal is the lowest validated lifetime cost for parts that assemble and perform reliably—not the most decimal places, the cheapest mold, or one perfect sample.
Technical sources and verification notes
ISO 20457:2026 — current published tolerance and acceptance framework for covered plastic molded parts; excludes stated surface imperfections.
ISO 294-4:2018 — molding and post-molding shrinkage of thermoplastic test specimens parallel and normal to flow.
ISO 291:2008 — standard atmospheres for conditioning and testing plastics; project acceptance conditions still require agreement.
ISO 14253-1:2017 — measurement-based conformity decision rules including uncertainty near specification limits.
ISO 1101:2017 y ASME Y14.5-2018 (R2024) — two major, distinct geometrical-tolerancing systems.
NIST process capability guidance — definitions and cautions for capability indices.
Protolabs tolerance guidance y BASF simulation guidance — supplier/manufacturer technical context, not universal capability or pricing tables.