Fits and Tolerances Using the Basic Hole System

Machine Design #29: Fits and Tolerances — How to Use the Basic Hole System

Two parts with the same nominal diameter of 20 mm can produce a loose fit, a close fit, or an assembly that cannot be installed by hand. The difference lies in the tolerance zones of the hole and shaft, not in the nominal dimension itself.

This article explains how to read fit designations, select a fit from the required function, and review the points that matter before placing a tolerance on a drawing. It is written from a practical design and machining perspective; it does not replace checking the current standard for the specific nominal size.

1. What problem do fits and tolerances solve?

In machine design, a hole-and-shaft pair usually needs to perform one of three tasks:

allow relative motion, such as a shaft rotating in a bushing;
locate parts accurately while still allowing disassembly;
hold parts firmly to transmit load or prevent movement.

If the drawing gives only the same nominal dimension for both the hole and shaft, the shop still does not know the permitted limits. Small variations caused by machining, temperature, coatings, and measurement methods can completely change the behavior of the assembly.

Fit tolerances define an allowable zone for both the hole and the shaft. The relationship between these zones determines the clearance or interference after assembly.

2. The three basic types of fit

2.1 Clearance fit

The hole is larger than the shaft in every possible combination of limit sizes. Clearance therefore always remains after assembly.

Use it when:

the parts must rotate or slide;
quick assembly and disassembly are required;
lubrication or thermal expansion needs space;
small alignment errors must be absorbed.

Too little clearance can cause seizure when temperature rises or a coating is added. Too much clearance increases vibration, noise, and positional error.

2.2 Transition fit

Depending on the actual manufactured sizes, the pair may have a very small clearance or light interference.

Use it when:

better location is required than a free-running fit can provide;
the assembly should still be removable with ordinary tools;
high torque is not transmitted solely through the fitted surfaces.

This is the fit range most easily misunderstood. The designer must define the assembly method, expected removal force, and any additional retention such as screws, keys, or retaining rings.

2.3 Interference fit

The shaft is larger than the hole in every possible combination of limit sizes. Assembly requires pressing, heating the outer part, or cooling the inner part.

Use it when:

torque or axial force must be transferred through the fitted surfaces;
the part must not move during operation;
the assembly will be disassembled rarely or not at all.

Interference must not be selected by experience alone. Check hoop stress, deformation, material, wall thickness, surface texture, assembly temperature, and the ability to control pressing force.

3. How to read a designation such as H7/g6

In the ISO system of limits and fits:

uppercase letters identify hole tolerance zones;
lowercase letters identify shaft tolerance zones;
the letter defines the position of the tolerance zone relative to the nominal-size line;
the number identifies the IT grade, where a smaller number generally means a narrower tolerance.

For example, H7/g6 combines an H7 hole tolerance zone with a g6 shaft tolerance zone. The designation alone does not give the deviations in micrometres: the nominal size and the applicable standard table are also required.

A common mistake is memorizing one designation and applying it to every diameter. Limit deviations change with the nominal-size range, so both the drawing and inspection plan must use the correct range.

4. Why is the basic hole system widely used?

In the basic hole system, the H tolerance zone of the hole is held as the reference. The type of fit is changed mainly by selecting a different shaft tolerance zone.

This is often economical because:

standard hole-making tools such as drills, boring tools, and reamers cannot be changed continuously for every fit;
shaft dimensions are usually easier to adjust by turning or grinding;
tool management and hole inspection remain simpler.

The basic shaft system is still useful when the shaft size is fixed by standard stock, a ready-made tie rod, a bearing, or another purchased component. In that case the shaft becomes the reference and the hole tolerance zone is varied.

A practical rule is to choose the system that makes production and inspection most stable, not the system used by habit on an old drawing.

5. A process for selecting a fit

Step 1: Define the function

Determine whether the pair must rotate, slide, locate, or transmit load. A location that must both position accurately and come apart for maintenance has different requirements from a permanent press fit.

Step 2: Evaluate the worst-case limits

Check both ends of the tolerance combination:

Is the minimum clearance sufficient to prevent seizure?
Does the maximum clearance compromise accuracy?
Can the maximum interference crack or distort the part?
Is the minimum interference sufficient to carry the load?

Step 3: Review real operating conditions

Is the assembly temperature different from the operating temperature?
Will the part be plated, anodized, painted, or surface-treated after machining?
Is the environment dusty, oily, clean, or corrosive?
Can the supplier repeatedly machine and measure the selected grade?

Step 4: Select the basic hole or basic shaft system

Prefer the basic hole system when standard tools create the hole and the shaft can be adjusted. Use the basic shaft system when the shaft dimension is constrained by a standard component or available material.

Step 5: Check the current standard

Use the correct nominal-size range in the table of tolerances and limit deviations. Do not copy a value from an old table or an online image without knowing its edition.

Step 6: Confirm machining and inspection

A tight tolerance without a suitable measurement method creates disputes rather than quality. Before release, agree on:

the final machining process;
the measurement equipment;
the reference temperature;
burr and coating treatment;
acceptance criteria.

6. Common design mistakes

Making every tolerance as tight as possible

Tighter tolerances increase the number of operations, measurement time, scrap rate, and cost. Tighten only to the level required by the function.

Ignoring surface treatment

A coating increases the shaft diameter and reduces the effective hole diameter. Define whether drawing dimensions apply before or after treatment.

Using an interference fit on a thin-walled part

Pressing force and hoop stress can distort the hole or crack the part. Check the material, wall thickness, and assembly method.

Ignoring temperature

Materials with different coefficients of thermal expansion can change the clearance significantly. An assembly that runs hot must be checked at operating temperature, not only at room temperature.

Specifying the designation without planning inspection

A standard-compliant designation does not by itself ensure manufacturability. Out-of-roundness, taper, and surface texture can make the real fit behave differently from a single-point diameter measurement.

7. Drawing-release checklist

Must the fit provide motion, location, or load transfer?
Have minimum and maximum clearance or interference both been checked?
Does the choice of basic hole or basic shaft system match the manufacturing process?
Is there a coating or heat treatment after machining?
Can operating temperature change the fit function?
Is the part wall sufficiently stiff for press fitting?
Are roundness, cylindricity, alignment, or surface-texture requirements also needed?
Does the shop have suitable inspection equipment?
Must the assembly come apart for maintenance?
Has the correct standard edition and nominal-size range been checked?

Conclusion

A fit is not merely a designation copied from an old drawing. It is a functional decision between two parts that also constrains machining, inspection, assembly, and maintenance.

Start from the function, evaluate both limit conditions, select the reference system that suits production capability, and only then consult the standard tables. When the drawing answers both “how will it assemble?” and “how will it be inspected?”, the tolerance reduces failures instead of merely making the drawing look precise.

Continue the tolerance series

View all MINATA technical articles