A clearance hole chart gives the hole diameter for a bolt or screw to pass through one part without engaging its threads. Select close, normal, or loose clearance from the required alignment, plate thickness, positional tolerance, washer size, coating, and assembly method. A 10-32 clearance hole is not a 10-32 tap drill: the former lets a #10 screw pass through, while the latter prepares material for cutting 10-32 internal threads. The chart below provides common starting values for metric and imperial fasteners, but the drawing and applicable standard control the final size.
What Is a Clearance Hole?
A clearance hole is larger than the fastener’s external thread diameter, so the bolt or screw can pass through the near part and clamp against a nut, tapped hole, or threaded insert in the far part. The hole does not provide thread engagement. Its purpose is to allow assembly while the clamped parts carry the load through friction, bearing, or a designed locating feature.
Clearance is different from a tap drill, pilot hole, counterbore, countersink, and reamed locating hole. A clearance hole can be intentionally close for alignment or larger for fast assembly and tolerance absorption. The required fit depends on whether the bolt is only a clamp or also serves as a locator.
For related fit decisions, see our guide to transition fits and mating feature control.
Clearance Hole Chart: Metric Sizes
| Bolt size | Nominal diameter (mm) | Close fit (mm) | Normal fit (mm) | Loose fit (mm) |
|---|---|---|---|---|
| M3 | 3.0 | 3.2 | 3.4 | 3.6 |
| M4 | 4.0 | 4.3 | 4.5 | 4.8 |
| M5 | 5.0 | 5.3 | 5.5 | 5.8 |
| M6 | 6.0 | 6.4 | 6.6 | 7.0 |
| M8 | 8.0 | 8.4 | 9.0 | 10.0 |
| M10 | 10.0 | 10.5 | 11.0 | 12.0 |
| M12 | 12.0 | 13.0 | 14.0 | 15.0 |
| M16 | 16.0 | 17.0 | 18.0 | 20.0 |
| M20 | 20.0 | 21.0 | 22.0 | 24.0 |
These metric values are practical reference ranges rather than a single mandatory standard. ISO or company tables may use different limits, especially for close fits, large diameters, countersunk screws, or coated fasteners. Specify the hole class and tolerance when the clearance affects alignment.
Clearance Hole Chart: Imperial Sizes
| Bolt size | Nominal diameter (in) | Close fit (in) | Normal fit (in) | Loose fit (in) |
|---|---|---|---|---|
| #4 | 0.112 | 0.116 | 0.120 | 0.125 |
| #6 | 0.138 | 0.142 | 0.147 | 0.156 |
| #8 | 0.164 | 0.169 | 0.177 | 0.187 |
| #10 | 0.190 | 0.196 | 0.201 | 0.218 |
| 1/4 | 0.250 | 0.257 | 0.266 | 0.281 |
| 5/16 | 0.3125 | 0.323 | 0.328 | 0.344 |
| 3/8 | 0.375 | 0.386 | 0.391 | 0.406 |
| 1/2 | 0.500 | 0.515 | 0.531 | 0.562 |
| 5/8 | 0.625 | 0.642 | 0.656 | 0.687 |
| 3/4 | 0.750 | 0.768 | 0.781 | 0.812 |
Imperial fasteners may be identified by fractional size, number size, or letter drill. The #10 row applies to the nominal external diameter of both common 10-24 and 10-32 screws; the pitch changes the threaded mating hole, not the clearance diameter. Always identify the full screw specification when the far part is tapped.
What Is a 10-32 Clearance Hole?
A 10-32 screw has a #10 nominal diameter and 32 threads per inch. A clearance hole for it is typically around 0.196 inch for a close fit, 0.201 inch for a normal fit, or 0.218 inch for a looser fit, subject to the chosen standard and tolerance. The hole should be large enough for the screw’s actual major diameter, plating, burr condition, and assembly variation.
Do not use a #21 drill, approximately 0.159 inch, as a 10-32 clearance hole. #21 is a common tap drill reference for cutting 10-32 threads in a separate part. Confusing these values creates a hole that the screw cannot pass through and may damage threads during assembly.
Close, Normal, and Loose Fits
Close clearance
Close clearance minimizes movement before clamping and can help a bolt pass through a controlled location. It needs accurate hole position, clean deburring, and consistent fastener dimensions. Use it when alignment matters and the parts can be assembled without forcing the bolt.
Normal clearance
Normal clearance balances easy assembly and reasonable alignment. It is a common choice for general brackets, covers, frames, and machine guards where the bolt clamps the joint rather than locates it.
Loose clearance
Loose clearance absorbs larger positional variation, coating buildup, forming variation, or field assembly conditions. It can speed installation but may allow visible movement, edge bearing, or washer exposure. Use a larger washer or a separate locating feature when the joint must remain aligned.
How Material and Finish Affect Hole Size
Laser cutting, punching, drilling, reaming, forming, anodizing, plating, and powder coating can all change the final hole. Punch clearance and sheet thickness affect edge quality. Bending can pull a hole out of position. Coatings add thickness and may reduce a previously acceptable clearance. Stainless steel work-hardening can make drilling difficult, while soft aluminum may raise a burr that narrows the effective opening.
State whether the clearance dimension applies before or after finishing. Mask or post-machine holes when coating buildup would interfere with assembly. For stainless or coated parts, inspect the actual finished hole rather than assuming the nominal cutting tool produced the final clearance.
Our sheet metal gauge and thickness guide helps connect thickness, forming, and hole placement decisions.
Hole Position, Edge Distance, and Washers
Diameter alone does not guarantee a reliable joint. Hole position must be referenced to functional datums, and edge distance must leave enough material for bearing and tear-out. A loose hole near an edge can weaken a flange even if the bolt passes freely. A washer should cover the clearance opening and distribute clamp load without overhanging the part.
- Check minimum edge distance for the material, bolt load, and washer outside diameter.
- Use a countersink or counterbore only when the fastener head requires it.
- Provide a flat seating surface so the washer does not rock on a bend or weld.
- Keep holes away from bend lines unless the forming process has been validated.
- Use dowels, shoulders, slots, or reamed holes when bolts alone cannot locate the assembly.
Design and Manufacturing Workflow
- Identify the fastener standard, nominal diameter, thread pitch, head style, and coating.
- Decide whether the hole is close, normal, or loose clearance based on assembly function.
- Check plate thickness, bend proximity, edge distance, washer coverage, and access.
- Select cutting, punching, drilling, or reaming based on quantity and tolerance.
- Define deburring, coating, masking, and whether dimensions apply before or after finish.
- Inspect diameter and position from functional datums, then perform a bolt-and-washer fit check.
This workflow prevents a common drawing error: copying a clearance value from a tap chart or choosing the smallest hole without checking actual assembly access.
Inspection and Quality Control
Measure clearance holes with calibrated pin gauges, plug gauges, bore gauges, optical measurement, or a micrometer depending on size and tolerance. Verify position with a CMM, height gauge, template, or functional fixture when the hole pattern controls assembly. Inspect burrs and edge damage because a nominal diameter can still fail if the bolt catches at the entry.
For first article inspection, record the tool, process, material, finish state, hole size, position, and fit result. In batch production, monitor punch or drill wear and coating variation. If a hole is near the lower limit, check it after deburring and finishing, not only immediately after cutting.
Supplier and Drawing Notes
- Call out “clearance hole for M6 bolt” or “clearance hole for #10-32 screw,” not only a drill size.
- State close, normal, or loose fit and the diameter tolerance.
- Identify whether the far part is tapped, uses a nut, or contains a threaded insert.
- Specify hole position, edge distance, countersink/counterbore, and burr limit.
- State coating, plating, forming, or passivation requirements that can change the finished hole.
- Define inspection gauges and whether a functional fastener fit is required.
Frequently Asked Questions
1. What is a clearance hole?
It is a hole larger than the fastener’s external thread diameter so a bolt or screw passes through without engaging threads in that part.
2. What is the difference between a clearance hole and a tap hole?
A clearance hole lets a fastener pass through. A tap hole, or tap drill hole, is smaller and prepares material for cutting or forming internal threads.
3. What is a 10-32 clearance hole size?
Common starting values are about 0.196 inch close, 0.201 inch normal, and 0.218 inch loose, but the governing clearance-hole standard and tolerance control the final choice.
4. Is a 10-32 tap drill the same as a 10-32 clearance hole?
No. A #21 drill near 0.159 inch is a common 10-32 cutting-tap reference; it is too small for a screw to pass through freely.
5. What is a normal clearance fit?
Normal clearance provides easy assembly with moderate positional allowance. It is common where the bolt clamps the joint but does not act as the locating feature.
6. When should I use a close clearance hole?
Use close clearance when bolt movement must be limited and the parts can be aligned accurately without forcing the fastener.
7. Do coatings change clearance holes?
Yes. Plating, powder coating, anodizing, and paint can add thickness or narrow the opening. Specify finished dimensions or mask and post-machine the hole.
8. Can a bolt clearance hole locate an assembly?
It can provide limited alignment, but ordinary clearance is not a precision locating system. Use dowels, shoulders, reamed holes, or designed locating features when position is critical.
9. How are clearance holes inspected?
Check diameter with pin or plug gauges and verify position from functional datums. A bolt-and-washer fit check can confirm assembly access but does not replace dimensional inspection.
10. What should a clearance hole callout include?
Include fastener standard and size, fit class or diameter tolerance, position, edge distance, countersink or counterbore, burr limit, finish state, and inspection requirement.
Related DAXIN Services
DAXIN supports CNC drilling, reaming, tapping, thread milling, sheet-metal punching and laser cutting, countersinking, deburring, coating coordination, CMM inspection, and first article reporting.
Final Thoughts
A clearance hole chart is most useful when it connects a fastener to the assembly function. Start with the exact metric or imperial bolt, choose close, normal, or loose clearance, then review position, edge distance, washers, finish, and inspection. For 10-32, keep the clearance-hole value separate from the much smaller tap-drill value. That simple distinction prevents avoidable fit and assembly failures.
Request a Clearance Hole Review
Send your drawing, fastener standard, material, thickness, finish, quantity, and inspection requirements to DAXIN CNC for a hole and assembly review.