Specifying limit tolerances isn’t just about hitting dimensional targets—it’s about making engineering decisions that prevent costly assembly failures and manufacturing delays. With decades of experience producing precision components for aerospace, medical, and audio applications, we’ve seen how smart tolerance specification separates successful products from expensive redesigns.
Specify limit tolerances by defining upper and lower dimensional boundaries directly on your drawing (e.g., 24.95-25.05mm) rather than using plus/minus notation. Focus tight tolerances only on critical functional surfaces, use standard tolerance grades where possible, and validate that your specified ranges match your supplier’s process capabilities.
Learn the decision-making framework that prevents over-specification, reduces manufacturing costs, and ensures your parts actually assemble as designed.
Table of Contents
Should You Specify Limit Tolerances or Let Dimensions Float?
Apply limit tolerances only when dimensional variation directly impacts assembly fit, product safety, or regulatory compliance. Most features perform identically whether they vary by ±0.05mm or ±0.2mm, so reserve tight specifications for genuinely critical interfaces and let standard machining capability handle the rest.
The decision usually becomes obvious when you think about what actually breaks if a dimension drifts. We’ve machined thousands of aluminum enclosures where customers initially wanted ±0.05mm on every radius and chamfer—but those decorative features work perfectly at ±0.2mm while the PCB mounting holes absolutely need ±0.1mm for proper alignment. Standard CNC processes naturally deliver ±0.1mm capability on most aluminum and steel features without special setups, verified through CMM inspection to ±0.005mm measurement uncertainty.
The real engineering insight comes from understanding interface requirements versus manufacturing convenience. Shaft fits need precise control because bearing performance depends on proper interference or clearance. Sealing surfaces require flatness specifications because gasket compression affects leak resistance. But internal clearance pockets, edge breaks, and tool access features rarely impact anything beyond manufacturing ease. Medical device housings following ISO 13485 require explicit tolerances on sealing interfaces, while audio equipment needs tight hole spacing for control alignment but flexible specifications elsewhere.
Design Takeaway: Focus specifications where function truly demands it—mating surfaces, safety-critical dimensions, and regulatory requirements. Let everything else float within standard ISO 2768-m capability to reduce cost and complexity.
Which Dimensions Need Limit Tolerance Specifications?
Use this 30-second screening method: specify limits only for holes that mate with other parts, surfaces that seal or bear loads, and any dimension appearing in regulatory standards. Skip everything else – decorative features, internal clearances, and non-contact surfaces can float within standard ±0.1mm machining capability without affecting performance.
Start with these five dimension types that always need specifications: bolt hole patterns and mounting interfaces, bearing seats and shaft fits, threaded hole depths, sealing surface flatness, and any dimension called out in safety or regulatory standards. These directly control assembly success or product safety. Everything else can use standard ISO 2768-m tolerances.
We’ve guided hundreds of projects using this rapid sorting approach. Audio equipment faceplates need tight hole spacing (±0.1mm) for control alignment, but edge chamfers work perfectly at ±0.2mm. Medical device housings require sealing surface flatness for gasket compression, while internal wire routing channels have no functional impact within normal machining variation. For parts with cost constraints, this method typically eliminates 70% of unnecessary tolerance callouts while preserving all critical performance requirements.
Priority ranking when you have multiple interface dimensions: first specify safety-critical features (pressure boundaries, structural connections), then assembly-critical features (bolt patterns, alignment pins), finally appearance-critical features (visible mating lines). Verification using CMM inspection to ±0.005mm measurement uncertainty ensures specified tolerances are actually achievable and measurable in production.
Validation Check:
| Question | If YES → | If NO → |
|---|---|---|
| If this varies ±0.2mm, does something break/not fit? | Specify limits | Use standard tolerance |
| Can I physically measure this feature? | Proceed with spec | Reconsider or redesign |
| Does my supplier machine similar features? | Safe to specify | Verify capability first |
Design Takeaway: Apply the five-category filter first, then run the three-question validation check. When specifications seem marginal, prototype one sample part to verify assembly fit before committing to production tolerances.
How Tight Should You Specify Your Limit Tolerance Range?
Use this decision tree: if your clearance gap is less than 0.2mm, specify ±0.05mm tolerance; if gap is 0.2-0.5mm, use ±0.1mm; if gap exceeds 0.5mm, standard ±0.2mm works fine. For interference fits, bearing manufacturers typically specify ±0.01-0.025mm depending on shaft size and application loads.
The decision becomes mechanical once you know your required fit. H7/h6 bearing fits need ±0.01-0.015mm to maintain proper interference without assembly damage. PCB mounting holes with standard 0.3mm clearance work perfectly at ±0.1mm—tighter serves no purpose and increases cost 30-50%. Sealing surfaces require ±0.05mm flatness for reliable gasket compression, while non-functional features perform identically at ±0.2mm standard capability.
Cost threshold guidance: If tolerance tightening adds more than 25% to part cost, evaluate design alternatives first. We’ve helped customers redesign problematic tight-tolerance features using larger clearances, self-aligning components, or adjustment mechanisms rather than expensive precision machining. For example, replacing a ±0.02mm alignment pin with a ±0.1mm pin plus spring-loaded adjustment reduced costs 40% with identical performance.
Material behavior affects these decisions significantly. Aluminum parts expand roughly 0.013mm per 10°C temperature rise on 50mm features—accounting for thermal effects prevents tolerance failures in service. Plastic components need 2-3x looser tolerances due to thermal movement and material creep over time.
Capability Verification:
| Tolerance Range | Required Cpk | Action Needed |
|---|---|---|
| ±0.1mm or looser | ≥ 1.0 | Standard verification |
| ±0.05–0.1mm | ≥ 1.33 | Process capability data |
| Tighter than ±0.05mm | ≥ 1.67 | Sample parts + FAI |
Safety Margin Calculation:
| Calculated Clearance | Design Target | Safety Factor |
|---|---|---|
| 0.1–0.2 mm | Add 50% | High precision needed |
| 0.2–0.5 mm | Add 25–30% | Standard safety margin |
| >0.5 mm | Add 10–20% | Generous clearance |
Design Takeaway: Validate tolerance decisions with supplier capability data and prototype testing. Build safety margins into clearance calculations rather than tightening tolerances to compensate for design uncertainty.
Can Your Supplier Meet Your Specified Limit Tolerances?
Before talking to suppliers, reality-check your tolerances: ±0.1mm is standard for most CNC work, ±0.05mm requires premium capability, and ±0.02mm needs specialized shops. Then test supplier knowledge by asking specific questions about measurement tools and process capability rather than accepting generic “yes we can do it” responses.
Quick tolerance reality check: If your part is aluminum and under 100mm, ±0.1mm is achievable at most shops. Tighter than ±0.05mm means finding specialized suppliers and paying 50-100% more. Steel parts can be held tighter than plastics. Large parts (over 200mm) are harder to hold tight than small ones. If your tolerance seems aggressive for the material and size, reconsider before shopping.
Questions that reveal real capability: “What measurement equipment do you use for ±0.05mm features?” Good shops mention CMMs, micrometers, or gauge pins. “Can you show me a similar part you’ve made?” Quality suppliers have examples readily available. “What’s your typical capability on aluminum parts this size?” Honest shops give ranges, not promises of perfection.
Cost benchmarks: Standard ±0.1mm work should quote at normal rates. Tolerances ±0.05mm typically add 30-50% to machining costs. Anything tighter than ±0.02mm often doubles costs and extends lead times. If quotes don’t reflect these realities, the supplier either doesn’t understand your requirements or can’t deliver them.
Red flags: Suppliers who don’t ask about part function, measurement requirements, or assembly context. Shops claiming universal capability without discussing equipment limitations.
Design Takeaway: Validate your tolerance expectations against material and size realities before supplier discussions. Test supplier knowledge with specific capability questions rather than accepting generic assurances.
How Do Limit Tolerances Affect Your Total Assembly Performance?
Focus tolerance analysis on your single most critical assembly dimension—usually the tightest fit or most important alignment. Count only the part tolerances that directly affect this dimension, add them up in the worst direction, then design clearances that accommodate this total variation.
Which tolerances actually matter: Start with your assembly’s biggest constraint—the gap that can’t be too small or the alignment that must be precise. Work backward from there. In a 20-part assembly, usually only 3-5 tolerances actually affect your critical dimension. Ignore tolerances that don’t impact your key requirement.
Minimum clearance guidelines: For slip fits needing easy assembly, design 0.2-0.5mm clearance after tolerance stack-up. For precision alignment with guided assembly, 0.1-0.2mm works. For interference fits, calculate based on material properties but typically need 0.02-0.1mm interference after accounting for variation.
Real example: Audio faceplate alignment required precise control spacing. Instead of analyzing all 15 part tolerances, we identified 4 tolerances affecting horizontal alignment and 3 affecting vertical. Adding worst-case values (±0.1mm each) gave ±0.4mm horizontal and ±0.3mm vertical variation. Designing 1.0mm clearance slots handled this variation perfectly.
When you have too many critical dimensions: Either redesign the assembly sequence to reduce tolerance chains, add adjustability through slotted holes or spring-loaded components, or accept that some features need tighter individual tolerances.
Design Takeaway: Identify your single most critical assembly dimension first, then focus tolerance analysis only on parts that directly affect it. Design clearances based on actual calculated variation, not arbitrary safety factors.
How Do You Know Your Limit Tolerances Are Too Restrictive?
When quotes come back significantly higher than expected, expensive tolerances are usually the culprit. Start by highlighting all dimensions tighter than ±0.05mm on your drawing, then eliminate any that don’t control mating surfaces or assembly fit. This rapid triage method typically reduces costs 40-60% by targeting the biggest cost drivers first.
The quickest way to find cost-killing tolerances involves checking each tight specification against actual function. Look at every ±0.02mm dimension and ask whether that surface touches another part during assembly. Internal corner radii, decorative chamfers, and non-contact features rarely justify precision tighter than ±0.1mm beyond ISO 2768-m general tolerance capabilities. These specifications often come from design habit rather than functional necessity, yet they create the steepest cost escalation during machining operations.
Priority ranking for maximum cost savings follows a predictable pattern across industries we’ve served, from medical device manufacturing under ISO 13485 to aerospace components meeting AS9100 requirements. Internal radii offer the biggest savings when relaxed, followed by non-mating hole positions, threaded depths, and external cosmetic features. Each change from ±0.02mm to ±0.05mm typically saves 30-50% on that feature’s machining cost, verified through CMM measurement at ±0.005mm uncertainty levels.
The two-minute design impact test works by imagining each tight tolerance at double its current value. Walk through your assembly mentally—do parts still fit together? Does anything critical fail? If you can’t identify a specific failure mode, the tolerance probably exceeds functional requirements. When three different shops quote similar high prices and suggest identical relaxations, they’re providing manufacturing reality based on their process capability data rather than trying to cut corners.
Design Takeaway: Target tolerances tighter than ±0.05mm on non-mating surfaces first for immediate cost relief. Use mental assembly testing to quickly validate whether relaxation affects function.
What's Your Backup Plan When Parts Exceed Limit Tolerances?
Out-of-specification parts need quick decisions based on what they actually control in your assembly. Deviations affecting mating surfaces like bearing bores or bolt patterns typically require rejection, while variations on internal non-contact features usually remain acceptable with proper evaluation.
The instant decision process starts with understanding what each dimension interfaces with during assembly. When your supplier calls reporting parts at ±0.08mm instead of ±0.05mm, identify whether that dimension controls a critical fit. Bearing bores need immediate rejection since precision fits affect performance, particularly when verified through calibrated measurement equipment. Bolt holes require checking whether fasteners still engage properly with the extra variation. Internal corner radii almost always remain acceptable since they don’t affect assembly or function within normal manufacturing variation.
Assembly impact evaluation involves adding the deviation to your clearance calculations using established quality control methods. If you originally designed 0.5mm clearance between components and the extra ±0.03mm variation reduces minimum clearance to 0.2mm, the parts probably still work. When deviation creates zero or negative clearance conditions, rejection becomes necessary to prevent assembly interference, documented according to standard quality system procedures.
Tolerance relief requests from suppliers need rapid evaluation based on feature function and manufacturing capability. Approve changes to internal features, threaded depths, and non-contact surfaces immediately since these rarely affect performance beyond ISO general tolerance ranges. Push back firmly on bearing surfaces, mating flanges, and sealing interfaces where precision matters for assembly success. For borderline cases, request sample parts verified through proper inspection methods to confirm actual fit before making production decisions.
Production delays often force emergency decisions with incomplete information, but documentation remains important for quality compliance. Accept deviations on any dimension that doesn’t control assembly fit, safety, or appearance requirements.
Design Takeaway: Base acceptance decisions on assembly interface requirements rather than drawing compliance. Focus rejection on mating surfaces while accepting deviations on internal and non-contact features.
Conclusion
Limit tolerance specification requires balancing functional requirements with manufacturing reality and cost constraints. Focus tight tolerances only on critical mating surfaces, verify supplier capability early, and design clearances that accommodate tolerance accumulation. Smart specification prevents costly over-engineering while ensuring reliable assembly performance.
Contact us to explore manufacturing solutions tailored to your product requirements.
Frequently Asked Questions
Calculate worst-case tolerance stack-up first. If three parts each contribute ±0.1mm variation, you need minimum 0.5mm design clearance (0.2mm + 0.3mm safety margin). Anything less risks assembly interference during production.
Yes, this is the most cost-effective approach. Specify tight tolerances (±0.05mm) only on mating surfaces like bearing bores or bolt patterns. Use standard ±0.1mm on everything else to minimize inspection complexity and machining costs.
Check your bearing manufacturer’s specifications. Most standard bearings work fine with ±0.025mm bore tolerance. Only precision spindle applications typically need ±0.01mm. When in doubt, ±0.025mm offers good performance at reasonable cost.
±0.05mm typically adds 30-50% to machining costs compared to ±0.1mm standard capability. The tighter tolerance requires slower feeds, more precise fixturing, and extended inspection time, making it worthwhile only for critical mating surfaces.
Add the extra ±0.03mm to your clearance calculation. If you designed 0.5mm clearance and now have 0.2mm minimum, probably still works. If you get zero or negative clearance, the parts won’t assemble reliably.
Ask which surfaces mate with other components. Approve changes on internal features immediately. For mating surfaces, request sample parts first to verify assembly fit before approving production changes.
