Tolerances are the invisible rules that govern whether a machined part fits, functions, and lasts. Yet they remain one of the most misunderstood and often misapplied aspects of precision manufacturing. Specify a tolerance too tight, and you inflate costs, extend lead times, and reject parts that would work perfectly. Specify one too loose, and assemblies fail, performance degrades, and customers complain.
This practical guide demystifies machining tolerances. You will learn what tolerances mean, how they are defined, how to select the right values for your application, and how to communicate them effectively to suppliers—saving money without compromising quality.
What Is a Machining Tolerance?
A tolerance is the allowable variation in a dimension. No manufacturing process can produce every part exactly at the nominal (target) value. Every cut, every movement, every measurement has inherent variability. Tolerances specify the acceptable range around the nominal.
Example: A shaft dimension is specified as 20.00 mm ±0.05 mm. That means the actual shaft diameter can be anywhere between 19.95 mm and 20.05 mm and still be acceptable.
Why Tolerances Are Necessary
- Process variability: Machine tools, tool wear, temperature changes, material variations all cause small deviations.
- Assembly requirements: Parts must fit together without binding or excessive looseness.
- Function: A bearing journal needs a precise fit; a clearance hole does not.
- Cost control: Tighter tolerances require slower machining, special tooling, more inspections, and higher scrap rates.
Types of Tolerances
1. Linear Tolerances
Apply to distances: lengths, widths, depths, heights.
- Bilateral tolerance: Variation on both sides of nominal (e.g., 50.00 ±0.10 mm).
- Unilateral tolerance: Variation on one side only (e.g., 50.00 +0.10 / -0.00 mm).
- Limit tolerance: Minimum and maximum values (e.g., 50.10 – 50.20 mm).
2. Angular Tolerances
Angles between features, typically in degrees (°) or minutes (‘). Common angular tolerance: ±0.5° for general machining; ±0.1° for precision work.
3. Geometric Dimensioning and Tolerancing (GD&T)
GD&T uses symbols to control the form, orientation, location, and runout of features. It is more powerful than linear tolerances for complex parts.
| Symbol | Control | Meaning |
|---|---|---|
| ⌒ | Flatness | Surface must lie between two parallel planes. |
| ⌭ | Circularity (roundness) | Every cross‑section must be within two concentric circles. |
| ∥ | Parallelism | Surface or axis must be parallel to a datum. |
| ⟂ | Perpendicularity | Surface or axis must be at 90° to a datum. |
| ⊕ | Position | Axis or center plane must lie within a cylindrical tolerance zone. |
| ⌔ | Concentricity | Axes of two features must be aligned (rarely used; position is often preferred). |
| Ⓜ | Maximum Material Condition (MMC) | Bonus tolerance when feature is at its largest material limit. |
Example: “The four holes shall be positioned within a 0.2 mm diameter cylindrical tolerance zone relative to datum A, B, and C at MMC.” This allows looser tolerances for holes that are slightly oversized, saving cost while ensuring assembly.
4. Surface Finish (Roughness)
Surface roughness is a form tolerance at microscopic scale. It is measured as Ra (average roughness) in micrometers (µm) or microinches (µin).
| Ra (µm) | Application | Typical Process |
|---|---|---|
| 12.5 | Rough machining, non‑functional surfaces | Sawing, rough turning |
| 3.2 – 6.3 | General machined surfaces | Turning, milling |
| 1.6 – 3.2 | Good finish for bearings, seals | Fine turning, grinding |
| 0.4 – 0.8 | Precision sliding surfaces | Grinding, honing |
| 0.1 – 0.2 | Mirror finish | Lapping, superfinishing |
Tolerance Grades and International Standards
Most engineering drawings reference ISO 286 (metric) or ANSI B4.1 (inch) tolerance classes.
ISO 286 Tolerance Grades (IT Grades)
IT grades from IT01 (tightest) to IT18 (loosest). For typical machining:
| Grade | Typical Application | Example (for 50 mm size) |
|---|---|---|
| IT5 | Precision gauges, high‑quality bearings | ±0.006 mm |
| IT6 | General precision machined parts | ±0.009 mm |
| IT7 | Good quality machining | ±0.015 mm |
| IT8 | Average machining, less critical | ±0.022 mm |
| IT9 | Coarse machining | ±0.035 mm |
| IT10 | Very coarse | ±0.055 mm |
Rule of thumb: IT6–IT7 is standard for most precision machined components. IT8–IT9 for non‑critical features. IT5 and tighter require grinding or lapping.
Fit Classes (Hole‑Shaft Systems)
- Clearance fit (e.g., H7/h6): Shaft always smaller than hole. Used for sliding or rotating assemblies.
- Transition fit (e.g., H7/k6): Shaft and hole may interfere slightly. Used for precise alignment.
- Interference fit (e.g., H7/p6): Shaft larger than hole; requires force or thermal assembly. Used for permanent mounting (gears on shafts).
The ISO system uses uppercase letters for holes (H, J, K, P, etc.) and lowercase for shafts (h, j, k, p, etc.). The number (6,7,8) indicates the IT grade.
Example: “50H7/g6” means a 50 mm diameter hole with H7 tolerance and a shaft with g6 tolerance, resulting in a sliding clearance fit.
How Tolerances Affect Manufacturing Cost
Many engineers specify unnecessarily tight tolerances “just to be safe.” This is one of the most expensive mistakes in machining.
Cost Drivers Related to Tolerances
| Tolerance Range | Relative Cost Factor | Explanation |
|---|---|---|
| Coarse (IT9–IT11) | 1.0x | Standard CNC turning/milling, no special measures. |
| Medium (IT7–IT8) | 1.2–1.5x | Slower feeds, more careful setups, more frequent tool changes. |
| Precision (IT5–IT6) | 2–4x | Requires grinding or fine boring; extra operations; 100% inspection. |
| Ultra‑precision (<IT5) | 5–10x | Lapping, special environment control; very slow. |
Why Tighter Tolerances Cost More
- Slower machining: To reduce variability, speeds and feeds must be reduced.
- Additional operations: You may need grinding instead of turning, or lapping instead of grinding.
- More setups: Multiple passes with intermediate measurements.
- Advanced metrology: CMM, air gauging, or optical inspection adds time.
- Lower yield: The probability of a part being out of spec increases exponentially as tolerance tightens.
- Tool wear management: Tools must be changed more frequently, adding cost.
The Law of Diminishing Returns
The cost of tightening a tolerance by half is often 3–5 times higher, not 2 times. Going from ±0.1 mm to ±0.05 mm may double the cost; going to ±0.025 mm may quadruple it.
Practical advice: Only tighten tolerances on features that truly need it. For all other dimensions, use the loosest tolerance that still allows the part to function.
How to Specify Tolerances on Drawings
Step 1: Use a General Tolerance Block
In the drawing’s title block or notes, define default tolerances for:
- Linear dimensions: e.g., “±0.1 mm for up to 100 mm, ±0.2 mm for 100–500 mm.”
- Angles: e.g., “±1°.”
- Radius / chamfer: e.g., “±0.2 mm.”
Example general tolerance note (ISO 2768‑m): “General tolerances per ISO 2768‑m (medium)”.
This standard automatically applies tolerances based on dimension range, freeing you from adding individual tolerances to every dimension.
Step 2: Apply Individual Tolerances to Critical Features
For dimensions that need tighter or looser control than the general block, add a specific tolerance next to the dimension.
Examples:
- “25.00 ±0.05”
- “Ø12.00 +0.02 / -0.00”
- “80.00 – 80.10”
Step 3: Use GD&T for Functional Requirements
Use GD&T symbols when the relationship between features is more important than the absolute size.
Example: Instead of specifying tight linear tolerances on the positions of four holes, use a positional tolerance at MMC. This often allows looser tolerances while still guaranteeing assembly.
Step 4: Add Surface Finish and Other Notes
- Specify roughness on critical surfaces (e.g., “Ra 1.6”).
- Define edge breaks (“BREAK ALL EDGES 0.2–0.5 mm”).
- Add deburring requirements (“REMOVE ALL BURRS 0.1 mm MAX”).
Common Tolerance Mistakes and How to Avoid Them
| Mistake | Consequence | Better Approach |
|---|---|---|
| Over‑tolerancing every dimension | High cost, unnecessary rejections | Use general block; only tighten critical features. |
| Ignoring GD&T | Hard‑to‑measure features, ambiguous control | Learn basics of position and profile tolerances. |
| Specifying unilateral tolerances without reason | Confusion, increased inspection cost | Use bilateral or limit unless assembly forces unilateral. |
| No surface finish callout | Unexpected rough or smooth surfaces | Add roughness values for functional areas. |
| Forgetting datum features | Inspection has no reference | Define primary, secondary, tertiary datums. |
| Using symmetrical tolerances for clearance holes | Unnecessarily tight | Use limit tolerances or MMC for holes. |
The Role of Process Capability (Cpk)
A tolerance is only useful if the manufacturing process can consistently achieve it. Process capability index (Cpk) measures how well a process holds tolerances.
| Cpk Value | Interpretation |
|---|---|
| < 0.67 | Process incapable; high defect rate. |
| 1.00 | 0.27% defects (acceptable for non‑critical). |
| 1.33 | 64 ppm defects (generally required for automotive). |
| 1.67 | 0.6 ppm (preferred for safety‑critical). |
Ask your supplier: “What Cpk can you achieve for my critical dimensions?” If they cannot provide data, consider qualifying them with a capability study.
Tolerances for Different Manufacturing Processes
Each process has inherent limits. Do not expect grinding tolerances from a simple turning operation.
| Process | Typical Linear Tolerance (±mm) | Surface Finish Ra (µm) |
|---|---|---|
| Band sawing / plasma cutting | ±1.0 – 3.0 | 12 – 50 |
| CNC turning (standard) | ±0.05 – 0.15 | 1.6 – 6.3 |
| CNC milling (standard) | ±0.05 – 0.15 | 1.6 – 6.3 |
| Turning (precision) | ±0.010 – 0.050 | 0.4 – 1.6 |
| Milling (precision) | ±0.010 – 0.050 | 0.8 – 3.2 |
| Grinding (cylindrical) | ±0.002 – 0.010 | 0.1 – 0.8 |
| Grinding (surface) | ±0.005 – 0.020 | 0.2 – 0.8 |
| Lapping / honing | ±0.001 – 0.005 | 0.05 – 0.2 |
| EDM (wire / sinker) | ±0.005 – 0.020 | 0.8 – 3.2 |
| Investment casting (as‑cast) | ±0.1 – 0.5 | 3 – 12 |
| Die casting (as‑cast) | ±0.05 – 0.15 | 0.8 – 3.2 |
Note: These are typical values. Advanced CNC machines and skilled operators can achieve tighter tolerances, but at higher cost.
Practical Tips for Buyers and Engineers
1. When in Doubt, Ask the Supplier
Share your design concept and ask: “What tolerances are realistic for this geometry and material?” A good supplier will suggest cost‑saving modifications.
2. Use the “10x Rule” for Inspection
Inspection equipment should be 10 times more precise than the tolerance being measured. For a ±0.05 mm tolerance, you need a gauge or CMM with at least 0.005 mm resolution.
3. Avoid “Stack‑Up” Problems
When multiple tolerances add up (e.g., chain dimensioning), the total variation can exceed the allowable gap. Use baseline dimensioning from a single datum.
4. Consider Material Effects
- Aluminum and plastics expand more with temperature; account for thermal expansion if parts will be measured at different temperatures.
- Heat‑treated steels can distort; specify tolerances after heat treatment, or allow extra stock for final grinding.
5. Specify Tolerances at Room Temperature (20°C / 68°F)
International standards assume measurement at 20°C. If your parts will be used at very different temperatures, discuss with your supplier.
Real‑World Example: Reducing Cost by Loosening Tolerances
Original drawing: A machined mounting plate with 40 holes, each hole individually toleranced to ±0.05 mm.
Problem: Suppliers quoted high prices due to extensive CMM inspection and slow machining. Scrap rate was 8%.
Analysis: Only 4 of the 40 holes were used for alignment; the rest were clearance holes for bolts.
Solution: Tight tolerance kept only on the 4 alignment holes (±0.05 mm). The other 36 holes were changed to “Ø12.5 ±0.5 mm” (much looser). General tolerance block applied to all other dimensions.
Result: Machining time reduced 30%, inspection time reduced 80%, scrap rate fell to 1%. Part cost dropped 25%.
Conclusion: Precision with Purpose
Tolerances are not a badge of honor; they are a design tool. The goal is not to achieve the tightest possible tolerance but to specify the minimum tolerance necessary for the part to function reliably in its assembly and environment.
By understanding the types of tolerances, the ISO system, the cost drivers, and the capability of different processes, you can create drawings that are both manufacturable and economical. And when you communicate clearly with your machining partner, you will get parts that fit, work, and keep your project on time and on budget.
