Bilateral Tolerance
Example: 20 ±0.05 mm. Use when variation in either direction is acceptable.
- Clear and widely understood
- Suitable for general structural dimensions
- Identify critical features separately
Choose the Right Tolerance Format
Define tolerances that meet functional, manufacturing and inspection needs. Tighten critical features without adding unnecessary cost to the rest of the part.
Unilateral Tolerance
Example: 20 +0.02/0 or 20 0/-0.02. Use when variation is allowed in only one direction.
- Useful for clearance or interference control
- Common for holes, shafts and locating 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 verify against inspection results
- Useful for precision fits and interchangeable parts
- Include the applicable fit standard where needed
Three Drawing Notes That Align Suppliers
- Unspecified linear and angular tolerances: ISO 2768-m or GB/T 1804-m.
- Hole-shaft fits: ISO 286, for example Ø20 H7/g6.
- Critical geometric relationships: GD&T per ISO 1101 or ASME Y14.5.
Set General Tolerances for Unspecified Dimensions
Use ISO 2768, GB/T 1804 or another stated standard to define allowable variation where individual dimensions are not toleranced.
Recommended Drawing Note
Add “Unspecified tolerances per ISO 2768-m” to the title block or technical requirements, then mark tighter tolerances on critical dimensions.
| Linear Size 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 to unspecified dimensions, not critical fits, locating features or sealing surfaces.
- State the selected ISO, GB or DIN standard and tolerance class for every supplier.
Specify IT Grades and Hole-Shaft Fits
An International Tolerance (IT) grade defines tolerance-zone width, while a fit code such as H7/g6 defines the hole and shaft relationship.
IT Grades: Lower Number, Tighter Tolerance
- IT5–IT6: High precision with demanding process and inspection controls
- IT7: Common for precision fits
- IT8–IT9: Common for structural parts and general assemblies
Fit Types: Clearance, Transition and Interference
- Clearance fit: easy assembly and removal
- Transition fit: accurate location 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 | Absolute tolerance generally increases with nominal size. |
| Ø50 mm | (Varies with size segment) | (Varies with size segment) | (Varies with size segment) | Confirm values from the applicable standard table for the diameter range. |
Typical Drawing Notes
- Hole: Ø20 H7, using the basic-hole system.
- Shaft: Ø20 g6, commonly used in a clearance fit.
- Also identify functional surfaces, datums and the inspection method.
Use GD&T to Control Functional Relationships
Geometric dimensioning and tolerancing (GD&T) controls form, orientation and location relative to defined datums without unnecessarily tightening every linear dimension.
Form
- Straightness and flatness
- Roundness and cylindricity
- Controls the shape of an individual feature
Orientation
- Parallelism, perpendicularity and angularity
- Controls orientation relative to a datum
- Define datums A, B and C where applicable
Location and Runout
- Position, concentricity and symmetry
- Circular and total runout
- Common for locating and rotating features
Inspection Feasibility Checklist
- Can deep-cavity or blind-hole features be measured by a coordinate measuring machine (CMM) or gauge?
- Is each datum stable, repeatable and resistant to clamping distortion?
- For tight runout requirements, are bearing seats, locating surfaces and machining setups controlled together?
Specify Surface Roughness by Function
Select Ra or Rz requirements for friction, sealing, fatigue, appearance and coating adhesion. Apply lower roughness only where the function requires it.
| 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 | Finer texture | Finish machining or optimized tool paths | Cosmetic or mating surfaces |
| Ra 0.8 | Smooth surface | Finish machining and light polishing | Sliding or pre-seal surfaces |
| Ra 0.4 and lower | Near-mirror finish | Polishing or mirror finishing | Mirror finishes and critical transparent-part surfaces |
Post-Processing Effects
- Sandblasting changes texture and may affect mating dimensions; mask or finish critical surfaces separately.
- Include paint, powder coating, plating or anodizing thickness in the tolerance budget for critical fits.
Check Assembly Tolerance Stack-Up
Analyze accumulated variation across the assembly chain so individually acceptable parts still assemble and function together.
Worst-Case Analysis
Use for safety-related, high-reliability or critical sealing requirements where every limit condition must assemble.
Total tolerance = |T1| + |T2| + |T3| + …
- Conservative and easy to verify
- May require tighter, more expensive component tolerances
Root Sum Square (RSS) Analysis
Use when production variation is stable and supported by data, with assembly performance managed statistically.
Total tolerance = √(T1² + T2² + T3² + …)
- Models statistical variation and yield
- Requires capable processes and measurement data
Assembly Chain Checklist
- Define the assembly datum and direct variation toward non-critical features.
- Use suitable clearances, chamfers and lead-ins.
- Concentrate tight tolerances on the critical closed-loop dimensions.
Reference Tolerances by Manufacturing Process
Use these values as early design and quotation references. Material, geometry, size, clamping, thermal behavior and inspection method determine the achievable project tolerance.
| 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 higher | Thin-wall deformation, clamping, temperature rise, tool path and inspection |
| Injection molding | ±0.10–0.30 mm | ±0.20–0.50 mm | Higher (needs evaluation) | Material shrinkage, wall thickness difference, warpage, mold temperature control and parameters |
| Sheet metal fabrication | ±0.10–0.20 mm | ±0.15–0.30 mm | Needs assessment | Bending springback, bending radius, hole margin, positioning datum and unfolding strategy |
| Vacuum casting | ±0.20–0.50 mm | ±0.30–0.80 mm | Not recommended for high accuracy | Material system, mold aging, batch stability and post-processing |
Where Tighter Tolerances May Be Needed
- Hole-shaft fits, repeatable positioning and sealing surfaces
- Runout that affects rotating performance
- Interchangeable assembly and consistent batch production
Where Tolerances May Be Relaxed
- Non-functional outlines
- Surfaces later covered by blasting or coating
- Assemblies that absorb variation through clearance or flexible features
Balance Tolerance Requirements and Cost
Tighter tolerances can add machining, setup, process-control and inspection work. Apply them only where they protect fit, sealing, positioning or function.
Why Costs Increase
- Longer cycles for finishing, correction and slower feeds
- More demanding fixtures and clamping control
- Additional CMM, gauge or full-inspection requirements
- Higher rework and scrap risk
Apply Tight Tolerances Where They Matter
- Individually tolerance critical fits, seals and locating features
- Use a general standard such as ISO 2768-m elsewhere
- Use GD&T for functional relationships
- Include coating thickness and post-processing distortion in the tolerance budget
Prepare Tolerances for Manufacturing and Inspection
Use these checks before submitting CNC machining, injection molding, sheet metal or vacuum casting drawings.
Drawing Strategy
- Give critical features explicit tolerances and datums
- Apply general tolerances to non-critical features
- Avoid one tight tolerance across the entire drawing
Inspection Access
- Provide measurement access for deep or hidden features
- Define go/no-go gauge requirements for critical holes
- State inspection methods and acceptance criteria
Assembly Robustness
- Add chamfers or radii where they support assembly
- Check stack-up and clearance budgets
- Use GD&T to define functional relationships
FAQs
Answers to common questions about default tolerances, fits, GD&T, surface roughness, inspection, cost and lead time.
±0.10 mm can be used as an initial reference for many CNC structural dimensions. The achievable tolerance depends on material, size, geometry, clamping and inspection. Identify critical holes, locating surfaces, seals and assembly dimensions for project-specific review.
Suppliers may apply different shop defaults, creating quotation and acceptance differences. State a standard such as ISO 2768-m or the applicable GB/T 1804 class, and tolerance critical fits, datums, seals and hole locations separately.
They are commonly used for unspecified dimensions on general structural parts, enclosures and brackets. Do not use them in place of explicit requirements for precision fits, locating holes, sealing grooves or bearing seats. Provide the part function and assembly relationship if the appropriate class is unclear.
Yes. A lower IT number defines a narrower tolerance zone and usually requires more process and inspection control. Use lower grades on features that affect interchangeability, clearance, sealing or positioning rather than across the entire drawing.
These ISO 286 codes define the tolerance-zone position and grade for a hole and its mating shaft. Together they determine the type of fit. Actual limits depend on nominal diameter, so provide a 2D drawing and the intended assembly function.
Use GD&T when function depends on form, orientation, position, runout or profile. It often defines assembly and inspection requirements more clearly than tighter linear dimensions. Include stable datums and the intended inspection method.
Yes. A lower Ra value may require finer tool paths, slower feeds or polishing. Apply the required roughness only to critical cosmetic, mating, sealing or sliding surfaces to control cost and lead time.
Worst-case analysis is appropriate when every limit condition must assemble. RSS is appropriate when process distributions are stable and supported by data. Define the functional clearance, datum path and closed-loop dimensions before selecting either method.
They can require more setups, slower machining, tighter tool control, additional inspection and greater rework or scrap risk. Concentrate tight tolerances on features that affect fit, movement, sealing, positioning or function.
Provide enough information to evaluate manufacturability, inspection, cost and lead time:
- 3D CAD files plus 2D drawings where available
- Material, quantity, application, project phase and target date
- Critical dimensions, fits, IT grades and GD&T requirements
- Datums, mating relationships, loaded features and sealing surfaces
- Surface roughness, finish and inspection-report requirements
Complete inputs support a more reliable review and quotation.
Already Have Drawings? Request a Custom Parts Quote
Upload your CAD files and add material, quantity, tolerance, finish and delivery requirements. We will review manufacturability and recommend the next step.