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.

RoughnessTypical appearanceTypical processCommon applications
Ra 3.2Visible machining textureStandard CNC finish or molded surfaceStructural and non-cosmetic surfaces
Ra 1.6Fine machining textureFinish machining or optimized toolpathsGeneral cosmetic and mating surfaces
Ra 0.8SmoothFinish machining with light polishingSliding surfaces and sealing preparation
Ra 0.4 or lowerNear-mirror finishFine polishing or mirror finishingMirror 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

FAQs