Clearance Hole Chart for Bolts & Screws (Inch & Metric)

* Not tabulated in ASME B18.2.8. The standard covers #0 through 1-1/2 inch but lists preferred sizes only, so #12, #14 and 9/16 are missing from inside its own range, and 1-3/4 and 2 inch fall past the top of it. These five rows are calculated, not published. MH29 p.1609 states the drill sizes were selected to give “as nearly as practical a step-patterned clearance size for the minimum recommended hole (Table 1b),” so each starred row is the nominal diameter plus the Table 1b allowance for its size range, rounded to the nearest standard drill; the same rule reproduces 64 of the 66 drill designations the standard publishes. 9/16, 1-3/4 and 2 inch land on exact fractional drills with no rounding; #12 and #14 round to the nearest number or letter drill, within 0.0024 inch.

† Maximum hole diameter on those rows is inferred. MH29 p.1609 states the hole tolerances for both inch and metric holes are ISO 286 class H12 close, H13 normal and H14 loose, so the maximum is the drill size plus that tolerance. B18.2.8 rounds the same thing into inches its own way. Measured against the 66 maximums it publishes, this matches 44 exactly and another 20 within 0.001 inch; the last two deviate by 0.002 and 0.005 inch. Even that worst case is immaterial on the upper limit of a clearance hole, but it is not the standard’s own number, so we note the discrepancy here.

* On the metric table the starred rows are the opposite case — published, not calculated. MH29 p.1610 notes its metric sizes agree with ISO 273 “except that ISO 273 covers fastener sizes M1 through M150,” so M3.5, M4.5, M7, M18, M22, M27, M33, M39, M45, M52, M60, M68, M76, M85 and M95 are taken from ISO 273:1979, whose fine, medium and coarse series are this table’s close, normal and loose. Maximum hole diameter is the drill size plus the ISO 286 tolerance ISO 273 assigns to each series — H12 fine, H13 medium, H14 coarse — with IT values from MH29 p.667, Table 4 (BS 4500:1969, the British adoption of ISO R286). For M1 through M1.4 and M105 through M150, see ISO 273 directly.

Published alternatives for the starred inch sizes, if you would rather use a tabulated value: MH29 p.2030, Table 4 lists clearance drills for #12 (Close Fit #2, 0.2210 in; Free Fit #1, 0.2280 in) and #14 (Close Fit D, 0.2460 in; Free Fit F, 0.2570 in), but in an older two-class Close/Free system that runs tighter than B18.2.8 — at 1/4 inch its Free Fit equals B18.2.8’s Close. MH29 p.1683, Table 5 lists 1-3/4 inch (Close 1-25/32, Normal 1-13/16) and 2 inch (Close 2-1/32, Normal 2-1/16) from the ANSI/ASME B18.3 socket head cap screw appendix, whose classes also run one step tighter than B18.2.8 at 1/2 inch and above. Neither system is interchangeable with this table’s columns — a value taken from either one is a class tighter than the heading it would sit under.

Common Clearance Hole Sizes

Normal fit is the one you want unless something specific says otherwise. In inch sizes, the clearance hole for a 1/4 bolt is a 9/32 in drill (0.281–0.290 in); for a 5/16 bolt, an 11/32 in drill (0.344–0.354 in); for a 3/8 bolt, a 13/32 in drill (0.406–0.416 in); for a 1/2 bolt, a 9/16 in drill (0.562–0.572 in); for a 5/8 bolt, an 11/16 in drill (0.688–0.698 in); and for a 3/4 bolt, a 13/16 in drill (0.812–0.824 in). A 9/16 bolt takes a 5/8 in drill, though that one is calculated rather than published — see the starred-size note above the table.

In metric, an M6 bolt takes a 6.6 mm drill (6.6–6.82 mm), an M8 takes 9 mm (9–9.22 mm), an M10 takes 11 mm (11–11.27 mm), and an M12 takes 13.5 mm (13.5–13.77 mm). Switch the table to Metric for the full M1.6 through M100 range, or pick a single fit class from the dropdown to see the hole diameter limits alongside each drill.

What Is a Clearance Hole?

A clearance hole — also called a through-hole, bolt hole, or pass-through hole — is a hole drilled larger than the fastener so the bolt or screw passes through the part without engaging threads. ASME B18.2.8-1999 (R2005) covers recommended clearance hole sizes for #0 through 1.5 inch and M1.6 through M100 fasteners in three classes of clearance: close, normal, and loose. The hole tolerances are based on ISO 286, using tolerance class H12 for close-fit, H13 for normal-fit, and H14 for loose-fit clearance holes.

How to Use This Clearance Hole Chart

Pick Inch or Metric, then find your nominal fastener size. The Nominal Drill Size column is the drill to put in the machine; Hole Dia Min and Hole Dia Max are the limits the finished hole must fall between. Use the Fit Class dropdown to narrow the table to one fit, or click “Hole Tolerances + More” to see the min and max limits for all three fits side by side. Click any value to copy it.

Bolting two plates with a bolt and nut means a clearance hole in both. If instead the screw threads into the lower part, that side gets a tapped hole — use the tap drill size chart for the tapped side. Once the joint is assembled, the bolt torque chart gives the tightening torque for the grade you are using.

We thread mill constantly at Pi Fabricators. You drill the hole first, then thread mill it — that is the only way to do it. The thread mill replaces the tap, not the drill. Our thread milling calculator computes the pitch diameter offset for that cut.

Example: Bolting a 3/8 in Bracket

You are bolting a steel bracket with 3/8-16 cap screws and the mounting holes are on a machined pattern, so the parts locate well. From the chart, the normal-fit clearance hole for 3/8 in is a 13/32 in drill, producing a hole of 0.406 in to 0.416 in. That gives 1/32 in of clearance over the 0.375 in fastener — enough to assemble without fighting the bolts.

If the same bracket were bolted to a weldment where hole positions drift, step to the loose fit: a 27/64 in drill, 0.422 in to 0.438 in, which gives 3/64 in of clearance. The tradeoff is that the bracket can sit off position by that much before you tighten it down, so only go loose when you need a lot of adjustment.

Clearance Hole Terminology

Close Fit

The tightest of the three. It suits a single fastener, or holes drilled at assembly or with matched tooling — cases where you already know the holes line up. Also worth it when there isn’t enough wall or edge distance left to give up to a bigger hole. Hole tolerance is ISO 286 class H12.

Normal Fit

The default, and what you want unless something specific says otherwise. It is sized for joints using two or more fasteners whose holes are made separately to ordinary tolerances, so it absorbs the usual drift — hole position, straightness, squareness to the face, center distances that do not quite agree between parts. Hole tolerance is ISO 286 class H13.

Loose Fit

The most generous. Use it when you need a lot of adjustment — hole patterns that don’t quite line up, weldments, anything you have to shift into position. Hole tolerance is ISO 286 class H14.

Nominal Drill Size

The recommended drill. For inch fasteners the drill sizes are tabulated by nominal drill designation as letter, number, or fractional sizes, selected to provide as nearly as practical a step-patterned clearance. For metric fasteners the minimum recommended hole is the drill size itself.

Hole Diameter Min / Max

The limits the finished hole must fall between. The minimum recommended hole is the drill size; the maximum recommended hole size is based on standard hole tolerances from the ISO System of Limits and Fits.

Frequently Asked Questions

Related Calculators

• Tap Drill Size Chart — UNC, UNF, and metric tap drill sizes with adjustable thread engagement
• Bolt Torque Chart — Recommended tightening torques for Grade 2, 5, and 8 bolts
• Drill Bit Size Chart — Decimal equivalents for number, letter, fractional, and metric drills
• Thread Milling Calculator — Pitch diameter offset for thread milling the tapped side of the joint