← AskMachinist · Guides · Calculator · 🔎 Search

Bolt Clearance Hole Sizes

Guide · Updated October 28, 2026

A clearance hole is the hole a bolt or screw passes through before it threads into a tapped hole or takes a nut. It is not a tap drill. How much bigger than the bolt it should be depends on how well the parts need to locate and how much hole position error has to be absorbed. ASME B18.2.8 for inch fasteners and ISO 273 for metric fasteners give three classes: close, normal and loose. The sizes below are taken from those tables.

Need an exact reference size?

Build any gage block stack with the free Gage Block Calculator. Free, no login.

Step by step

Know the bolt size: Use the nominal diameter. Thread pitch does not change the clearance hole, so 1/4-20 and 1/4-28 use the same hole.
Pick a fit class: Close for accurate location and small heads, normal for general assembly, loose for coated bolts, weldments or several holes that must line up.
Read the chart: Find the nominal drill for that size and class.
Check position tolerance: With floating fasteners, the position tolerance is about the hole minus the bolt diameter; make sure the drawing tolerance works with the class you chose.
Check head bearing: A larger hole leaves less material under the head; use a washer on loose holes in soft material.
Drill and deburr: Spot drill first so the hole lands where it should, then deburr both sides.

Inch clearance holes (ASME B18.2.8)

#4: close #31 (0.120 in), normal #30 (0.128 in), loose #27 (0.144 in)
#6: close #23 (0.154), normal #18 (0.170), loose #13 (0.185)
#8: close #15 (0.180), normal #9 (0.196), loose #3 (0.213)
#10: close #5 (0.206), normal #2 (0.221), loose B (0.238)
1/4: close 17/64 (0.266), normal 9/32 (0.281), loose 19/64 (0.297)
5/16: close 21/64 (0.328), normal 11/32 (0.344), loose 23/64 (0.359)
3/8: close 25/64 (0.391), normal 13/32 (0.406), loose 27/64 (0.422)
1/2: close 17/32 (0.531), normal 9/16 (0.562), loose 39/64 (0.609)
5/8: close 21/32 (0.656), normal 11/16 (0.688), loose 47/64 (0.734)
3/4: close 25/32 (0.781), normal 13/16 (0.812), loose 29/32 (0.906)
1: close 1-1/32 (1.031), normal 1-3/32 (1.094), loose 1-5/32 (1.156)

Values are the minimum hole diameters listed with the nominal drills in ASME B18.2.8. A drilled hole usually runs a little over drill size, which the standard allows for in its maximum diameters.

Metric clearance holes (ISO 273)

M3: fine 3.2 mm, medium 3.4 mm, coarse 3.6 mm
M4: 4.3, 4.5, 4.8 mm
M5: 5.3, 5.5, 5.8 mm
M6: 6.4, 6.6, 7.0 mm
M8: 8.4, 9.0, 10.0 mm
M10: 10.5, 11.0, 12.0 mm
M12: 13.0, 13.5, 14.5 mm
M16: 17.0, 17.5, 18.5 mm
M20: 21.0, 22.0, 24.0 mm

ISO 273 calls the classes fine, medium and coarse. ASME B18.2.8 uses the same metric values and calls them close, normal and loose.

How to choose the fit

Close fit is used when the bolt helps locate the part, when a socket head screw sits in a counterbore with little room, or on small precision fixtures. It needs good hole position, because there is little room for error.

Normal fit is the default for most machined parts. Loose fit suits large weldments, painted or galvanized bolts, and patterns of many holes drilled in separate parts. If two parts must locate accurately, use dowel pins and normal clearance holes rather than counting on close-fit bolts to locate.

Worked example: floating fastener tolerance

Two plates are held with 1/4-20 bolts and nuts, normal fit holes of 0.281 in. With a floating fastener, the position tolerance available is about T = H − F = 0.281 − 0.250 = 0.031 in diameter for each part. If the drawing calls position 0.014 in diameter on each plate, the parts will assemble with room to spare.

If you switched to close fit (0.266 in), T = 0.016 in, so a 0.014 in position callout leaves very little margin and the holes need to be spot drilled on a CNC or jig bored.

Worked example: fixed fastener tolerance

A cover is held with M6 screws into tapped holes in a housing, medium fit 6.6 mm holes in the cover. For a fixed fastener, the total tolerance H − F = 6.6 − 6.0 = 0.6 mm is shared between the clearance hole and the tapped hole, so each part might get 0.3 mm diameter position tolerance. If the tapped hole is long, add projected tolerance zone thinking, because a tilted thread moves the screw at the top of the cover.

Common problems

Using a tap drill size for a clearance hole, choosing close fit on parts drilled on a manual mill with no DRO, forgetting that paint and plating shrink the hole, and using a loose hole under a small screw head with no washer in aluminum. Check a drilled hole with a pin gage set if a drawing gives a hole tolerance.

FAQ

What size hole for a 1/4 bolt?

Normal fit is 9/32 in (0.281). Close fit is 17/64 (0.266) and loose fit is 19/64 (0.297) per ASME B18.2.8.

What size hole for an M6 screw?

6.6 mm is the ISO 273 medium (normal) fit; 6.4 mm is fine and 7.0 mm is coarse.

Does thread pitch change the clearance hole?

No. The hole is based on the nominal diameter.

How do I check a hole size?

Use pin gages or a small hole gage, and check the gage on gage blocks; build stacks free at gageblockcalc.com.

Related guides and calculators

Build your stack in seconds

The free Gage Block Calculator finds the fewest-block combination for inch and metric sets, with wear blocks. No login.

Questions? Ask a machinist.

General shop information only — follow your drawing, tool maker's data and your quality system.