ISO Fit Symbols Explained: H7/g6, H7/h6 and More

Introduction

ISO fit symbols combine a letter and a number to define the tolerance zone for a hole or shaft. The letter identifies where the tolerance zone sits relative to the nominal dimension, while the number identifies the applicable ISO tolerance grade. For example, H7/g6 combines an H7 hole with a g6 shaft to create a controlled clearance fit commonly used for shafts, bushings, bearings, and other mating components.

Understanding these symbols helps engineers define functional clearance, alignment, assembly, and interchangeability requirements before a part reaches production. This guide explains what common ISO fit symbols mean, how hole and shaft tolerance zones work, and how nominal diameter affects the resulting limits.

1. What Do the Letters f, g, h, js, k, m, and n Mean in ISO Fits?

These letters define the position of a tolerance zone in relation to the nominal, or basic, size. ISO 286 assigns each letter to a specific position above, below, or across the zero line.

Common Shaft Tolerance Positions

• f and g: The shaft tolerance zone is below the nominal size and is commonly used to create clearance.
• h: The upper deviation is zero, and the shaft tolerance zone extends below the nominal size.
• js: The tolerance zone is distributed approximately equally around the nominal size.
• k, m, and n: The tolerance zone moves progressively above the nominal size and may create a transition or interference fit, depending on the mating hole and nominal diameter.

Common Hole Tolerance Positions

• H: The lower deviation is zero, and the hole tolerance zone extends above the nominal size. It is the most commonly used hole-basis tolerance position.

Think of the letter as the vertical position of the tolerance band on a chart. The number identifies the width of that band according to the applicable ISO tolerance grade.

2. What Is the ISO System of Limits and Fits, and How Does It Differ from ANSI?

The ISO system uses hole-basis or shaft-basis methods with letter-and-number tolerance class symbols. For example, H7/g6 combines an H7 hole with a g6 shaft. The permitted limits are selected from standard tables according to the nominal diameter.

By contrast, ANSI inch-based fit systems may use fit classifications such as RC for running and sliding fits, LC for locational clearance fits, LT for locational transition fits, and FN for force and shrink fits.

Important: ISO and ANSI fit classes are not automatically interchangeable. Any comparison must account for nominal size, required clearance or interference, operating conditions, material, temperature, assembly method, and the applicable standard.

3. Why Does the Hole-Basis System Usually Use H?

Many common manufacturing tools, including drills, reamers, and boring tools, are used to produce standardized hole sizes. Designers can therefore establish the hole as an H tolerance class and vary the shaft tolerance position to obtain the required fit.

Advantages of the Hole-Basis System

• Improved component interchangeability
• More practical use of standardized hole-making tools
• Reduced manufacturing complexity and tooling cost
• Multiple fit conditions can be created by changing the shaft tolerance class

Common hole-basis combinations include:

• H7/h6: Close clearance or locational clearance fit
• H7/g6: Controlled clearance or sliding fit
• H7/js6 or H7/k6: Transition-fit conditions, depending on size and limits
• H7/p6: Interference or press fit

4. ISO Shaft Tolerances: h6, g6, and Related Fit Classes

Shaft tolerance symbols specify the position and width of the permitted shaft-size range. The result cannot be determined from the letter and number alone; the nominal diameter range must also be known.

What Does an h6 Shaft Tolerance Mean?

An h6 shaft tolerance places the upper deviation at the nominal size while the permitted tolerance extends below nominal. The numerical limits depend on the nominal diameter range specified by ISO 286 and must be verified for the applicable part size.

When an h6 shaft is paired with an H7 hole, the theoretical minimum clearance may be zero because both tolerance zones meet at the nominal size. The actual fit remains dependent on the permitted hole and shaft limits.

What Does a g6 Shaft Tolerance Mean?

A g6 shaft tolerance places the entire shaft tolerance zone below the nominal size. When combined with an H7 hole, it commonly creates a controlled clearance fit. Actual minimum and maximum clearance depend on the nominal diameter range.

This controlled clearance can support applications requiring reliable assembly, accurate location, or low-friction movement without the force required for an interference fit.

How Do h6 and g6 Differ?

• h6: The maximum permitted shaft size reaches the nominal dimension.
• g6: The maximum permitted shaft size remains below the nominal dimension.
• H7/h6: Can provide zero theoretical minimum clearance.
• H7/g6: Maintains positive theoretical clearance throughout the permitted limits.

5. What Does an H7/g6 Fit Mean in Real-World Dimensions?

Consider a nominal hole-and-shaft diameter of Ø20 mm.

Using the applicable ISO 286 diameter range, the example limits are:

• H7 hole: 20.000 mm to 20.021 mm
• g6 shaft: 19.980 mm to 19.993 mm

The resulting clearance is:

• Minimum clearance: 20.000 − 19.993 = 0.007 mm
• Maximum clearance: 20.021 − 19.980 = 0.041 mm

In practical terms, the shaft remains slightly smaller than the hole throughout the specified tolerance limits. This permits assembly without force while maintaining controlled clearance.

H7/g6 is therefore commonly described as a sliding or controlled-clearance fit. It can be suitable for rotating shafts, pins, bushings, sleeves, and other mating components where easy assembly and limited play are required.

In production, this is where precision CNC machining becomes critical. Even when the fit symbol is correct on the drawing, the final result still depends on material behavior, machining strategy, inspection method, surface finish, and the consistency with which the tolerance is maintained across multiple parts. Engineering and procurement teams in Dallas–Fort Worth can review our precision CNC machining services in Dallas for custom metal and engineering-plastic parts.

For shafts, pins, bushings, sleeves, and other cylindrical components, CNC turning services should be evaluated against the required fit, surface finish, material, geometry, and inspection method.

6. How Are ISO Fits Selected Based on Function?

The appropriate fit depends on how the mating components must assemble, move, locate, transmit load, and perform under operating conditions.

Use clearance fits when relative movement or straightforward assembly is required. Use transition fits when accurate location is important and a small amount of clearance or interference is acceptable. Use interference fits when the joint must resist movement and will be assembled by pressing, heating, cooling, or another controlled method.

For CNC machined parts used in assemblies, the selected fit should be reviewed together with the mating component, tolerance stack-up, surface finish, material, operating temperature, assembly method, and inspection requirements before production begins.

For a practical method of selecting between clearance, transition, and interference fits, see our guide to choosing the right ISO fit for real-world design.

7. How Are Tolerance Values Determined from ISO Fit Symbols?

Tolerance bands and limit deviations are defined through the ISO 286-1 and ISO 286-2 standards. Production limits should be obtained from the applicable standard tables or verified engineering references.

The fit symbol provides three essential pieces of information:

• Capital or lowercase letter: Identifies whether the tolerance class applies to a hole or shaft.
• Letter: Establishes the position of the tolerance zone relative to nominal size.
• Number: Establishes the tolerance grade and therefore the width of the tolerance zone for the applicable nominal-size range.

For the Ø20 mm example:

• H7: 0 / +0.021 mm, producing a tolerance width of 0.021 mm
• g6: −0.020 / −0.007 mm, producing a tolerance width of 0.013 mm

The hole and shaft limits can then be compared to determine the minimum and maximum possible clearance or interference.

8. How Does Shaft or Hole Size Affect the Tolerance Band?

Nominal diameter directly affects the numerical tolerance limits. Even when the same tolerance class—such as H7 or g6—is used, the permitted tolerance generally becomes wider as the nominal diameter range increases.

For this reason, “H7/g6” by itself is not enough to define final manufacturing limits. The nominal diameter and applicable ISO 286 size range must also be specified and verified.

9. What Is the Impact of Choosing the Wrong Fit?

Tolerances may appear to be small decimal values on a drawing, but an incorrect fit can create significant assembly, reliability, maintenance, and production costs.

If the Fit Is Too Tight

• Assembly damage or excessive installation force
• Seized or restricted moving components
• Distortion of the shaft, hole, bearing, or surrounding features
• Cracking or failure caused by excessive interference
• Problems resulting from thermal expansion

If the Fit Is Too Loose

• Wobble or loss of concentricity
• Misalignment between mating components
• Noise and vibration
• Reduced positional accuracy
• Premature bearing, shaft, gear, or assembly failure

The fit should therefore be selected according to function, load, movement, lubrication, material, operating temperature, assembly process, service conditions, and inspection capability.

10. Common ISO Fits and Their Typical Applications

The following combinations illustrate commonly referenced hole-basis fits. The final selection must be verified for the nominal diameter, materials, operating conditions, assembly method, and applicable standard requirements.