Getting tolerances right in sheet metal fabrication prevents costly assembly failures and manufacturing delays. With decades of experience fabricating enclosures, brackets, and chassis for aerospace, medical, and industrial applications, small tolerance adjustments can dramatically improve both fit and cost-effectiveness.
Tolerances in sheet metal work differently than machined parts. Bending introduces stress, forming creates springback, and thin materials are prone to distortion. Understanding these realities helps you specify dimensions that actually work in production while avoiding unnecessary costs from over-tolerancing non-critical features.
Learn realistic sheet metal tolerances, how to avoid assembly issues, and when to adjust specs for the best balance of cost and performance.
Table of Contents
What's a realistic tolerance for holes, slots, or bend angles in sheet metal?
Standard sheet metal tolerances are ±0.2mm for holes/slots and ±1-2° for bend angles. Tighter tolerances (±0.1mm) require secondary machining and increase costs by 25-40%. Use the table below to select appropriate tolerances based on material thickness and feature type.
Material Thickness Punched Holes Bend Angles Secondary Machining Required
0.5–1.5mm ±0.15–0.2mm ±2–3° For tolerances <±0.1mm
1.5–3mm ±0.1–0.2mm ±1–2° For tolerances <±0.1mm
3–6mm ±0.2–0.3mm ±1–1.5° For tolerances <±0.15mm
From our experience with medical device enclosures and aerospace brackets, we consistently achieve ±0.15mm on mounting holes using progressive dies in 2mm aluminum. However, stainless steel above 2.5mm thickness typically requires ±0.25mm to prevent excessive tool wear and maintain production rates. Small holes (under 6mm diameter) in thin materials often distort during punching, making secondary drilling necessary for tight tolerances.
ISO 2768-m provides standard tolerances for non-critical dimensions: ±0.5mm for lengths up to 30mm. Medical applications following ISO 13485 often require ±0.1mm on sealing surfaces, necessitating CNC machining after forming operations.
Cost impact is significant: moving from ±0.5mm to ±0.2mm adds 15-25% to fabrication cost due to tool precision requirements. Specifying ±0.1mm typically doubles the cost for those features as secondary machining becomes necessary.
Design Takeaway: Reserve ±0.1-0.2mm tolerances for functional features like mounting holes and mating surfaces. Use standard ±0.5mm tolerances elsewhere to minimize cost. When tolerances tighter than ±0.15mm are required, specify machined holes rather than attempting tight-tolerance punching.
How do tolerances affect whether my parts will actually fit during assembly?
Poor tolerance planning causes 60-80% of sheet metal assembly failures, primarily from inadequate clearances between mating parts and misaligned fastener holes. As a general rule, fastener holes need 0.3-0.5mm total clearance to accommodate ±0.15mm part tolerances, while sliding fits require 0.2-0.4mm clearance for smooth operation without binding.
Assembly Type Part Tolerance Required Clearance Fastener/Feature
M3–M5 fasteners ±0.15mm 0.3–0.4mm Standard screws
M6–M10 fasteners ±0.2mm 0.4–0.6mm Structural bolts
Sliding interfaces ±0.1mm 0.2–0.3mm Drawer slides, covers
Housing joints ±0.2mm 0.5–1.0mm Welded corners
The most common failure we see involves hole patterns where engineers specify ±0.2mm positioning but only provide 0.2mm clearance around fasteners. This creates a 50% chance of assembly problems since the tolerance and clearance are nearly equal. A safer approach uses the 2:1 rule – if your parts have ±0.2mm tolerances, provide at least 0.4mm clearance.
Individual part variations affect different assembly types differently. Bend angle variations of ±2° on a 50mm flange translate to ±1.7mm positioning error at the tip, often exceeding available fastener clearance. For sliding interfaces like covers or panels, even ±0.15mm variations can cause binding if clearances are insufficient.
Consider using slotted holes when single-part positioning uncertainty exceeds half your available clearance. Round holes work well when part tolerance is ±0.1mm and you have 0.4mm clearance, but switch to slots when tolerance approaches 0.2mm with similar clearance. We typically slot one direction and maintain round holes perpendicular to prevent over-constraint.
For separately fabricated parts that must mate, establish common reference datums on your drawings. Two brackets that both reference the same mounting surface will align better than brackets dimensioned from their own edges, preventing individual manufacturing variations from compounding during assembly.
Design Takeaway: Use the 2:1 clearance rule (clearance = 2x tolerance) for fastener holes, specify slotted holes when part tolerance exceeds half your clearance, and establish common datums when parts must align precisely.
How does tolerance stack-up affect my overall assembly accuracy?
Tolerance stack-up multiplies individual part errors across multi-part assemblies, creating total variations 2-4x larger than any single part tolerance. A 3-part assembly with ±0.2mm individual tolerances produces ±0.6mm worst-case or ±0.35mm statistical variation at the final interface – often exceeding available clearances and causing assembly failures.
Here’s how to calculate stack-up for a typical 3-part mounting system:
Example: Base plate → mounting bracket → spacer
- Part A: ±0.2mm
- Part B: ±0.2mm
- Part C: ±0.2mm
Worst Case: 0.2 + 0.2 + 0.2 = ±0.6mm total Root Sum Square: √(0.2² + 0.2² + 0.2²) = ±0.35mm total
As assembly complexity increases, stack-up grows rapidly. A 4-part system with the same ±0.2mm individual tolerances creates ±0.8mm worst-case variation, while a 5-part assembly reaches ±1.0mm total error. This exponential growth explains why simple assemblies work reliably while complex multi-part systems often experience fit problems.
Stack-up becomes problematic when total variation approaches your clearance limits. We’ve measured actual assemblies where 4-part chassis systems with individual ±0.15mm tolerances created 1.2mm final positioning errors, preventing fastener engagement despite each part meeting specifications.
The solution lies in dimensioning strategy. Avoid “chain dimensioning” where each feature references the previous one – this mathematically adds all tolerances together. Instead, use “baseline dimensioning” where all critical features reference a single common datum, eliminating tolerance accumulation between parts.
Angular stack-up compounds the problem exponentially. Multiple bent parts with ±2° individual tolerances can create severe misalignment at assembly interfaces, especially over longer spans where small angular errors translate to large linear displacements.
Use worst-case calculations for safety-critical assemblies and RSS methods for general production planning. Most sheet metal operations follow statistical distributions, making RSS appropriate for cost-effective design decisions.
Design Takeaway: Calculate stack-up before finalizing designs using RSS for typical assemblies and worst-case for critical functions. Use baseline dimensioning from common datums, and limit assembly chains to 3-4 parts when precise positioning is required.
Will tight tolerances cause problems during sheet metal bending or forming?
Yes, tight tolerances on bend-adjacent features often cause cracking, distortion, or dimensional instability during forming operations. Features within 2x material thickness of bend lines typically shift ±0.1-0.3mm during bending, while springback creates 1-3° angular variations.
Quick Check Rule: Measure distance from bend line to any critical feature. If less than 4x material thickness, expect tolerance problems. Example: 2mm aluminum = keep features 8mm+ from bends.
The most common issue involves pre-punched holes near bend lines. We’ve measured 0.3mm position shifts in 3mm stainless when holes were just 5mm from 90° bends. The forming forces literally relocate features beyond specified tolerances.
When tight tolerances are required near bends: Form first, then machine critical features using bent geometry as reference. Alternatively, design formed features (tabs, embossed details) rather than punched holes – they maintain better accuracy during bending operations.
Material selection matters significantly. Aluminum maintains predictable behavior, while stainless steel work-hardens unpredictably and shifts features more dramatically during forming.
Design Takeaway: Keep precise features 4x+ material thickness from bend lines. When unavoidable, plan secondary operations or use formed features instead of pre-punched holes.
Which dimensions need tight control vs. standard tolerances?
Apply tight tolerances only to functional features – mounting holes, sealing surfaces, user interfaces – while using standard tolerances (±0.5mm) everywhere else. This selective approach reduces costs 20-30% while maintaining all necessary performance.
80/20 Decision Rule:
- Circle mounting holes, mating surfaces, user-contact areas → tight control needed
- Mark overall dimensions, internal features, hidden edges → standard tolerances fine
- Focus precision where it affects assembly, function, or appearance
Feature Type Tolerance Strategy Why
Mounting holes ±0.1–0.15mm Assembly fit
User interfaces ±0.1–0.2mm Quality perception
Hidden features ±0.5mm standard No functional impact
Real example: Audio equipment faceplate – ±0.1mm on control holes (user feels precision), ±0.2mm on display window (visible quality), ±0.5mm on overall panel size (no impact). Result: perfect function, 25% cost reduction.
Production volume affects cost impact dramatically. Prototypes see immediate penalties from over-tolerancing, while high-volume runs can justify precision tooling investments.
Design Takeaway: Start with standard tolerances everywhere, then tighten only features affecting assembly, user experience, or function. This prevents costly over-specification while ensuring quality where it matters.
Can I loosen my tolerances to reduce fabrication cost or lead time?
Yes, loosening non-critical tolerances from ±0.1mm to ±0.2mm typically reduces costs 15-25%, while moving to standard ±0.5mm tolerances can cut fabrication costs by 30-50%. Lead times also improve since looser tolerances eliminate secondary operations, reduce setup complexity, and lower scrap rates from marginal parts.
Systematic tolerance review process: Start with overall part dimensions – these rarely affect function and offer immediate savings. Next, examine internal cutouts, reliefs, and non-mounting holes. Finally, review bend angles and cosmetic edges. Leave mounting holes, sealing surfaces, and user interfaces until last since these typically need tight control.
Cost Impact by Tolerance Level:
- ±0.05mm: Requires CMM inspection, secondary machining (+100% cost)
- ±0.1mm: Precision tooling, careful setup (+40-60% cost)
- ±0.2mm: Standard precision operations (+15-25% cost)
- ±0.5mm: Normal shop tolerances (baseline cost)
Real optimization example: Medical enclosure drawing originally specified ±0.1mm on overall housing dimensions (60mm x 40mm), ±0.1mm on internal wire routing slots, and ±0.1mm on mounting holes. We relaxed housing dimensions to ±0.5mm and internal slots to ±0.3mm while keeping mounting holes at ±0.1mm. Result: 35% cost reduction with zero functional impact.
Safe-to-loosen features: Overall part dimensions, internal cutouts for wire routing, cosmetic bend radii, non-critical hole diameters, and aesthetic edge treatments. These typically have no assembly or functional requirements that justify tight tolerances.
Never loosen these: Mounting hole positions, threaded features, sealing groove dimensions, mating surface profiles, and any dimension that affects part-to-part fit or user interaction. The cost savings disappear if assembly problems occur.
Supplier collaboration tip: Send your drawing to fabricators and ask “Which tolerances are driving the cost on this part?” Experienced shops immediately identify over-specified features and can suggest specific relaxations that maintain function while reducing price.
Use this risk assessment: If loosening a tolerance by 2-3x (±0.1mm to ±0.3mm) creates no assembly or functional problems, it’s safe to relax. If you’re unsure, start with 50% relaxation (±0.1mm to ±0.15mm) and evaluate the cost benefit.
Design Takeaway: Review each tight tolerance systematically and ask “Does this dimension affect fit, assembly, or user experience?” Loosen everything that doesn’t, starting with overall dimensions and working toward functional features. Collaborate with suppliers early to identify cost-driving tolerances.
Conclusion
Smart tolerance specification balances precision with cost-effectiveness – reserve tight control for functional features while using standard tolerances elsewhere. Consider material behavior, bend proximity, and assembly requirements when making tolerance decisions to avoid costly manufacturing problems.
Contact us to explore sheet metal fabrication solutions tailored to your product requirements.
Frequently Asked Questions
Use the 2:1 rule – if your parts have ±0.2mm tolerances, provide at least 0.4mm clearance around fasteners. For M3-M5 screws with ±0.15mm part tolerances, 0.3-0.4mm clearance works well. For M6+ bolts with ±0.2mm tolerances, use 0.4-0.6mm clearance to ensure reliable assembly without binding.
Keep any features requiring precise positioning at least 4x material thickness away from bend lines. For 2mm aluminum, this means 8mm minimum distance. Features closer than this will experience stress-related distortion during forming that can shift positions by ±0.1-0.3mm, exceeding most tolerance requirements.
Yes, systematically review each dimension starting with overall part sizes, then internal features, finally mounting holes. Moving from ±0.1mm to ±0.2mm typically saves 15-25%, while relaxing to ±0.5mm can reduce costs 30-50%. Never loosen tolerances on mounting holes, sealing surfaces, or features affecting assembly fit.
Use Root Sum Square (RSS) method for most applications: √(tolerance₁² + tolerance₂² + tolerance₃²). For a 3-part assembly with ±0.2mm individual tolerances, RSS gives ±0.35mm total variation. Use worst-case addition (0.2 + 0.2 + 0.2 = ±0.6mm) for safety-critical assemblies or when statistical analysis isn’t appropriate.
Apply tight tolerances (±0.1-0.2mm) only to mounting holes, mating surfaces, sealing grooves, and user-interface features. Use standard tolerances (±0.5mm per ISO 2768-m) on overall dimensions, internal cutouts, cosmetic edges, and any feature that doesn’t affect assembly or function. This approach reduces costs 20-30% while maintaining quality.
For most sheet metal parts, ±0.2mm is achievable with standard tooling and processes. Going tighter than ±0.1mm often requires secondary machining or specialized fixturing, which increases cost by 40-60%. We recommend tolerancing only critical features tightly and keeping others at ISO 2768-m levels for cost efficiency.
