Manufacturing Tolerances & Standards Guide

How to Specify Clear, Manufacturable Tolerances

A useful tolerance supports part function, can be produced consistently and can be inspected reliably. Apply tight limits only where the design requires them.

Bilateral Tolerance

Example: 20 ±0.05 mm. Use when equal variation above and below the nominal size is acceptable.

Clear and widely understood
Suitable for many general structural dimensions
Identify critical features separately

Unilateral Tolerance

Example: 20 +0.02/0 or 20 0/-0.02. Use when variation is acceptable in only one direction.

Controls clearance or interference in one direction
Common for hole, shaft and positioning features
Define the datum and inspection method

Limit Dimensions

Example: 19.98–20.02 mm. Use when the acceptable upper and lower limits must be explicit.

Easy to inspect against stated limits
Useful for precision fits and interchangeable production parts
Reference ISO 286 when a standardized fit is required

Recommended Drawing Notes

Unspecified linear and angular tolerances: ISO 2768-m or the selected equivalent standard.
Hole-shaft fits: ISO 286, for example Ø20 H7/g6.
Critical geometric relationships: GD&T per ISO 1101 or ASME Y14.5.

General Tolerances: ISO 2768 and GB/T 1804

A stated general-tolerance standard gives suppliers one default rule for dimensions without individual tolerances and reduces inconsistent interpretation.

Recommended Drawing Statement

State "Unspecified tolerances per ISO 2768-m" in the title block or technical notes, then mark stricter requirements on critical dimensions.

Linear dimension range (mm)	Fine f (reference)	Medium m (reference)	Coarse c (reference)
0.5 – 6	±0.05	±0.10	±0.20
>6 – 30	±0.10	±0.20	±0.50
>30 – 120	±0.15	±0.30	±0.80
>120 – 400	±0.20	±0.50	±1.20
>400 – 1000	±0.30	±0.80	±2.00

Avoid Misuse

General tolerances apply only where no individual tolerance is shown. Mark critical fits, sealing surfaces and positioning features separately.
For international supply chains, state the selected ISO, GB or DIN standard and tolerance class explicitly.

IT Grades and Hole-Shaft Fits per ISO 286

The IT grade defines tolerance-zone width, while a fit such as H7/g6 defines the hole and shaft tolerance positions. Together they control clearance, interference and interchangeability.

IT Grade: Tolerance-Zone Width

IT5–IT6: high precision with demanding process and inspection control
IT7: commonly used for precision fits
IT8–IT9: commonly used for structural parts and general assemblies

Fit Types

Clearance fit: easy assembly and disassembly
Transition fit: accurate positioning with controlled assembly
Interference fit: secure retention by press or thermal fitting

Example diameter	IT6 (reference)	IT7 (reference)	IT8 (reference)	Engineering note
Ø20 mm	≈ 0.013 mm	≈ 0.021 mm	≈ 0.033 mm	For the same IT grade, the absolute tolerance generally increases with diameter.
Ø50 mm	(Varies with size segment)	(Varies with size segment)	(Varies with size segment)	Use the applicable ISO 286 table or an approved tolerance calculator for the exact value.

Drawing Examples

Hole: Ø20 H7, using the common hole-basis system.
Shaft: Ø20 g6, commonly paired with H7 for a clearance fit.
Also identify the functional datum and inspection method.

Geometric Dimensioning and Tolerancing (GD&T)

When function depends on position, orientation or runout, GD&T can express the requirement more clearly—and often more economically—than tightening every linear dimension.

Form

Straightness and flatness
Roundness and cylindricity
Controls the shape of an individual feature

Orientation

Parallelism, perpendicularity and angularity
Controls feature orientation relative to a datum
Identify datums A, B and C where required

Location and Runout

Position, concentricity and symmetry
Circular runout and total runout
Critical for many rotating and locating features

Inspection Feasibility Checklist

Can deep-cavity or blind-hole features be reached by a coordinate measuring machine (CMM) or gage?
Is each datum stable and repeatable without clamping distortion?
For tight runout or concentricity, are bearing seats, locating surfaces and machining setups controlled together?

Surface Roughness: Ra, Rz and Functional Performance

Select roughness for friction, sealing, fatigue, coating adhesion and appearance. A smoother surface is not automatically better and usually costs more.

Roughness	Typical appearance	Typical process	Common applications
Ra 3.2	Visible machining texture	Standard CNC finish or molded surface	Structural and non-cosmetic surfaces
Ra 1.6	Fine machining texture	Finish machining or optimized toolpaths	General cosmetic and mating surfaces
Ra 0.8	Smooth	Finish machining with light polishing	Sliding surfaces and sealing preparation
Ra 0.4 or lower	Near-mirror finish	Fine polishing or mirror finishing	Mirror finishes and critical transparent-part surfaces

Finishing Allowances

Sandblasting changes texture and can affect mating dimensions; mask functional surfaces or finish them afterward when needed.
Include paint, plating and anodizing thickness in the tolerance budget for critical mating surfaces.

Assembly Tolerance Stack-Up: Worst Case vs. RSS

Dimensions accumulate across an assembly chain. Stack-up analysis helps prevent assemblies from failing even when every individual part is within specification.

Worst Case

Use for high-reliability applications where every allowed dimensional extreme must still assemble, such as safety features or critical seals.

Total tolerance = |T1| + |T2| + |T3| + …

Conservative and easy to verify
May require tighter, more expensive component tolerances

RSS (Statistical Stack-Up)

Use for controlled production processes when statistical distributions and assembly yield are supported by reliable process data.

Total tolerance = √(T1² + T2² + T3² + …)

Often reflects real production variation more closely
Requires process-capability and inspection data

Assembly-Chain Design Priorities

Define assembly datums so variation is directed toward non-critical dimensions.
Use appropriate clearances, chamfers and lead-ins to improve assembly robustness.
Concentrate tight tolerances on the critical links in the closed-loop chain.

Process Tolerance Capability by Part Size

Use these ranges only for early design discussion. Actual capability depends on material, geometry, thermal effects, tooling, setup and inspection; critical dimensions require project-specific engineering review.

Process	≤100 mm (reference)	100–500 mm (reference)	≥500 mm (reference)	Key influencing factors
CNC Machining	±0.10 mm	±0.20 mm	±0.30 mm or wider	Thin-wall distortion, clamping, thermal effects, toolpath and inspection
Injection Molding	±0.10–0.30 mm	±0.20–0.50 mm	Project review required	Material shrinkage, wall-thickness variation, warpage, mold temperature and process settings
Sheet Metal Fabrication	±0.10–0.20 mm	±0.15–0.30 mm	Project review required	Bend springback, bend radius, edge distance, locating datum and flat-pattern strategy
Vacuum Casting	±0.20–0.50 mm	±0.30–0.80 mm	Not suited to high precision	Material system, mold aging, batch consistency and finishing

When Tighter Tolerances Are Justified

Hole-shaft fits, repeatable positioning and sealing contact
Runout or concentricity that affects rotating performance
Interchangeable assemblies with demanding batch consistency

Where Tolerances Can Often Be Relaxed

Non-functional profiles and cosmetic contours
Surfaces later covered by blasting or coating
Assemblies that absorb variation through clearance or compliant features

Why Tighter Tolerances Increase Cost

Tighter tolerances can require slower machining, more stable setups, closer temperature and tool-wear control, additional inspection and lower yield. Apply them only to function-critical features.

Main Cost Drivers

Longer cycles for finishing, re-cuts and slower feed rates
More complex tooling and sensitive clamping
Additional CMM, gage or full-inspection requirements
Higher rework and scrap risk

Focus Precision Where It Matters

Specify critical fits, seals and locating features individually
Apply general tolerances such as ISO 2768-m elsewhere
Use GD&T for functional relationships instead of tightening every size
Include coating thickness and finishing distortion in the tolerance budget

Best Practices for Manufacturable, Inspectable Assemblies

Use these checks during design review for CNC-machined, molded, sheet-metal and vacuum-cast parts.

Drawing Strategy

Give critical features tight tolerances and clear datums
Use general tolerances for non-critical dimensions
Avoid applying one tight tolerance to the entire drawing

Inspectability

Provide accessible measurement surfaces for deep or hidden features
Consider go/no-go gages for critical holes
Define the inspection standard and method

Assembly Robustness

Add chamfers or radii where they support assembly
Analyze stack-up and clearance budgets
Express functional relationships with GD&T

Need a project-specific tolerance review?

Share your 3D model or drawing for process, material and assembly-based feedback with quotation and lead-time review.

Get an Instant Quote Contact an Engineer