How do I know which dimensions on my part require tight tolerances?
How Do I Know Which Dimensions on My Part Require Tight Tolerances?
Direct Answer: Trace Every Tight Requirement to a Functional Consequence
A dimension needs a tight tolerance when variation could cause a defined failure in fit, location, motion, sealing, load transfer, safety, or a required verification test. Start from the assembly and work backward through the mating features and datum system. Do not tighten a feature merely because it appears precise or belongs to a regulated product. For each candidate characteristic, record its failure mode, mating condition, operating range, stack contribution, manufacturing state, and measurement method; loosen it only after the design authority confirms that the risk remains controlled.
When Tight Tolerances Are Justified
1. Functional Fits and Mating Surfaces
Fit requirements belong to the complete mating pair and operating condition. Select the fit system, nominal size, tolerance class, surface texture, geometry, temperature, lubrication, and assembly method together. Examples:
Shaft and hole fits: under the ISO limits-and-fits system, H7/g6 is commonly a clearance fit in the basic-hole system, not a press fit and not a symmetric plus/minus tolerance. Choose the hole and shaft zones from the required minimum and maximum clearance or interference at the nominal size.
Locating holes: specify size for the pin fit and geometric location relative to functional datums. A plus/minus coordinate tolerance and a position tolerance are different controls and should not be treated as interchangeable numerical ranges.
Threaded interfaces: identify the governing thread system and designation, such as a metric ISO tolerance class or a Unified thread class. Select the required gauge or measurement method from that system; do not combine ISO and ANSI class labels into one generic grade.
In robotic actuators, linkages, or surgical tools, a fit can affect backlash, binding, leakage, preload, or replaceability. The RFQ should include the mating drawing, assembly process, operating temperature, load direction, lubrication or seal, and the result that constitutes failure.
2. Moving or Load-Sensitive Assemblies
For sliding or rotating systems, allocate tolerance from permissible variation in clearance, alignment, load distribution, vibration, and thermal growth:
Position: use a geometric position control when the feature axis or center plane must lie within a defined tolerance zone relative to stated datums, or when a pattern's internal relationship is being controlled. Choose material-condition modifiers and datum references only when they represent the functional requirement.
Flatness and perpendicularity: flatness controls a surface independently of a datum, while perpendicularity controls orientation relative to a datum. Derive each value from contact, sealing, bearing, optical, or assembly need; no universal value applies by industry label or surface length alone.
3. Stack-Up in Multi-Part Assemblies
A tolerance stack should follow the functional loop from one assembly interface to the other. Include dimensions, geometric effects, clearances, compliant elements, coatings, thermal expansion, and assembly shifts. Then allocate available variation to controllable contributors:
Stack height: use worst-case analysis when every permitted extreme must assemble, or an approved statistical method when production distributions, independence assumptions, and risk policy justify it. Do not divide the total equally without considering process and sensitivity.
Surface relationship: control parallelism, runout, or profile only where it protects shaft alignment, seal compression, bearing load, valve motion, or another named function. Connect the callout to datums that reproduce how the part is located in assembly.
4. Regulatory Compliance Dimensions
Standards and quality systems affect tolerancing in different ways. Read the applicable product and drawing requirements instead of assigning dimensions from a certification name:
AS9100 defines aerospace quality-management-system requirements; it does not prescribe a universal set of aerospace critical dimensions. ISO 2768 supplies general tolerances only when properly invoked and within its stated scope.
Medical device ISO 13485 addresses a quality-management system; it does not define a class of “validated surfaces.” Product risk management, design outputs, process validation where required, and acceptance criteria determine controlled characteristics.
UL and IEC publications contain product- and test-specific requirements, not one general tolerance table for every EV battery casing. Identify the exact edition, clause, construction, test setup, and customer requirement before deriving a dimension.
A standard-driven characteristic should cite the governing document and revision, feature or drawing note, acceptance method, and required record. If the connection cannot be shown, treat the numerical limit as a design assumption that needs review.
Efficient Tolerancing: What to Loosen
Feature Type | Suggested Tolerance |
|---|---|
Cosmetic features | Define a visual zone, reference sample, viewing condition, permitted edge or blend variation, and only the dimensions needed for neighboring interfaces. |
Non-critical holes | Size and locate from fastener clearance, tool access, drainage, or ventilation needs; do not use locating-hole controls when the hole establishes no assembly position. |
Logo surfaces | Use marking artwork, orientation, visible boundary, depth or contrast, and cosmetic acceptance instead of precision geometry unrelated to branding. |
Chamfers, radii | Define the edge function: burr removal, handling safety, mating lead-in, stress reduction, seal protection, or coating coverage. Allocate precision only where that function needs it. |
Loosening a nonfunctional requirement can reduce special tooling, slow finishing passes, inspection programming, and rejection exposure. The change is valid only after checking nearby interfaces, datum use, finish buildup, assembly tools, and visual boundaries. Record approved changes on the controlled drawing rather than leaving them as supplier assumptions.
Supplier Deliverables for a Tolerance Review
For a supplier review through the DFM process, ask the supplier to return:
A marked drawing linking every proposed tight characteristic to its setup, manufacturing datum, tool access, material state, and delivered condition.
A list of requirements that appear disconnected from fit, motion, sealing, load, appearance, or compliance, with the cost or process consequence of retaining them.
Alternative GD&T, fit, or datum proposals written in the drawing's governing ISO or ASME system and submitted to the design authority for approval.
A characteristic-level inspection proposal, including CMM inspection only when availability, probe access, alignment, uncertainty, and reporting are confirmed for the order.
Perform tolerance-stack analysis early for multi-part assemblies and sealed enclosures. Provide mating drawings, bearings or seals, fastener and locating strategy, coatings, assembly sequence, load and temperature range, and permitted functional variation. The design owner should approve the allocation before suppliers optimize individual parts.
RFQ Checklist for Deciding Which Dimensions Need Tight Tolerances
Build a characteristic matrix before requesting tight-tolerance pricing: feature, function, failure mode, mating part, datum, nominal size, tolerance or geometric zone, material state, finish state, measurement method, and required record. For FAI reporting, state the required format and characteristic coverage instead of assuming it is included. Add project-specific requirements for aerospace, medical, and automation parts. Approve a tight value only when the functional allocation, manufacturing route, and measurement decision are all explicit.
