The bolt hole is half of every bolted joint, and it is the half that decides whether assembly is pleasant or a fight. Two charts cover it: ISO 273 for metric screws M2–M30 in all three fits, and ASME B18.2.8 normal fit for #4 through 1-inch bolts — plus the fit-selection logic, drill choices, and the floating-fastener formulas that turn a hole size into a real tolerance call.
ISO 273 defines three hole series per screw size — fine, medium, and coarse — as the minimum hole diameter for the screw to pass through. “Medium” is the everyday fabrication value and the default in most CAD hole tables; the nominal screw size never appears as its own hole diameter because a bolt needs real clearance to function.
| Screw | Fine (mm) | Medium (mm) | Coarse (mm) |
|---|---|---|---|
| M2 | 2.4 | 2.6 | 2.9 |
| M3 | 3.2 | 3.4 | 3.6 |
| M4 | 4.3 | 4.5 | 4.8 |
| M5 | 5.3 | 5.5 | 5.8 |
| M6 | 6.4 | 6.6 | 7.0 |
| M8 | 8.4 | 9.0 | 10 |
| M10 | 10.5 | 11 | 12 |
| M12 | 13 | 13.5 | 14.5 |
| M16 | 17 | 17.5 | 18.5 |
| M20 | 21 | 22 | 24 |
| M24 | 25 | 26 | 28 |
| M30 | 31 | 33 | 35 |
Typical tolerance
Close ≈ H12, medium and coarse ≈ H13. The tolerance band sits on top of the minimum hole — an M8 medium hole is ⌀9H13 (+0.22/0).
Countersunk screws
Hole diameter is unchanged; the countersink angle and depth come from the screw head standard (ISO 2009/2010 for 90° heads) — see the hex & nut dimensions guide for head sizes.
Heavy coating
Hot-dip galvanized stacks commonly add 1–2 mm to the hole; ISO 273 coarse plus 1 mm is a defensible starting point, verified against the coating spec.
ASME B18.2.8 defines normal, close, and loose fits for unified screws; the normal column below is the default for machine design. The same hole fits both thread pitches of a size — a #10 hole is identical for 10-24 and 10-32, because clearance rides on the major diameter, not the pitch.
| Screw | Normal (in) | mm equiv. | Drill bit to grab |
|---|---|---|---|
| #4 | 1/8″ | 3.2 | Letter F (0.257) is close; 1/8″ is the normal fractional |
| #6 | 5/32″ | 4.0 | 5/32″ twist drill |
| #8 | 11/64″ | 4.4 | 11/64″ twist drill |
| #10 | 13/64″ | 5.2 | 13/64″ twist drill |
| 1/4 | 17/64″ | 6.7 | 17/64″ — between letter H and I |
| 5/16 | 21/64″ | 8.3 | 21/64″ |
| 3/8 | 25/64″ | 9.9 | 25/64″ |
| 1/2 | 33/64″ | 13.1 | 33/64″ (or 13 mm ≈ 0.5118″) |
| 5/8 | 41/64″ | 16.3 | 41/64″ |
| 3/4 | 49/64″ | 19.4 | 49/64″ (or 19.5 mm) |
| 7/8 | 57/64″ | 22.6 | 57/64″ |
| 1 | 1-1/16″ | 27.0 | 1-1/16″ (or 27 mm) |
mm equivalents are the fractional value converted; where a metric drill sits within 0.1 mm, it is listed as a practical substitute. For the full close and loose series, ASME B18.2.8 Table 2 is the governing source.
A clearance hole is a tolerance decision, not a lookup reflex. The three ISO 273 series exist because different assemblies pay for position accuracy in different currencies — alignment, cost, or field forgiveness.
+0.2 to +0.4 mm over nominal
Precision locations, dowel-located assemblies, parts aligned by the bolts themselves. Minimal float — expect to ream or jig-bore for repeatable results.
+0.5 to +1.0 mm over nominal
The default for most fabricated assemblies and the value punch-press tooling produces. Enough float to absorb hole-position tolerance without starving bearing area.
+1.0 to +2.0 mm over nominal
Rough fabrications, castings, welded frames, field assembly with mismatch risk. Also the right choice for painted or galvanized stacks where the coating eats clearance.
A clearance hole size is a minimum; GD&T turns it into an assembly guarantee. Two formulas cover every bolted configuration, and they are the fastest sanity check on whether a drawing’s hole callout can actually assemble.
Floating fastener — both parts have clearance holes
H = F + T_max
The fastener “floats” in both parts. H = minimum hole diameter, F = maximum fastener diameter, T_max = the sum of the positional tolerances (at MMC) on the holes in both mating parts. Every micron of position error in either part must be absorbed by the hole’s clearance.
Fixed fastener — one part threaded, one drilled
H = F + 2T
The screw’s position is now fixed by the threaded part, so the drilled part alone must absorb the fit — its positional tolerance gets half the budget. This is why bolt-hole patterns on castings threaded in-place need tighter position callouts than the same pattern on two drilled plates.
Worked example: M6 screws (F = 6.0 max) through two plates with a chosen medium hole of 6.6 mm. Floating: T_max = 6.6 − 6.0 = 0.6 mm total position — split as ±0.21 mm per part at MMC, comfortable for punched holes. Fixed into a threaded boss: T = (6.6 − 6.0)/2 = 0.3 mm for the drilled plate alone. Same hole, very different tolerance conversation — which is exactly why the two formulas stay separate.
The hole is a tolerance decisionPhoto: UnsplashBonus tolerance makes this friendlier than it looks: a hole drilled at ⌀6.9 instead of the 6.6 minimum earns its position an extra 0.3 mm of allowed error. Clearance and position trade directly — which is the entire point of the formulas.
The single most common hole-tolerance mistake on fabrication drawings is calling a bolt hole H7. H7 is the tightest of the everyday hole classes — a locating tolerance for dowels, bushings, and bearing seats where the part must not move relative to the hole. A bolt is the opposite: its job requires freedom to shift so the threads can clamp instead of the shank bearing on the hole wall.
ISO 273 pairs each fit series with a broad IT-grade tolerance: close-fit holes at H12, medium and coarse at H13. For the M8 medium hole that means ⌀9.0 H13 — a +0.22/0 mm band. H13 on a drilled hole is achievable with a standard twist drill; H12 usually wants reaming. Compare that to H7 on the same ⌀9.0 hole: a +0.015/0 band, five-plus times tighter, at five-plus times the cost, buying a bolt-fit that is worse, not better.
The one-line rule
H7 = the part is located by the hole. H12/H13 = the bolt is located by the hole, loosely. If your assembly needs the second thing — and bolted joints always do — write the ISO 273 fit on the drawing and let the hole chart do its job. When a designer reaches for H7 on a bolt hole, what they usually actually want is a dowel, and the dowel has its own standard.
One nuance keeps the rule honest: precision assemblies that use fitted bolts (reamed shanks, hexagon fit bolts per DIN 1434/1435) genuinely do locate by the bolt shank, and those get H7-class holes by design. They are the exception that proves the rule — and they say so explicitly on the drawing, because nothing about a standard hex bolt implies it.
M5 takes 5.3/5.5/5.8 mm and M6 takes 6.4/6.6/7.0 mm across the three fits. Sheet-metal enclosures almost always run the medium column in punched holes; the 0.4–0.6 mm of clearance is what lets a punch-tolerance panel still assemble to a machined boss. For 3D printing or laser cutting, jump one column — process variability, not design intent, sets the real hole.
The trio covers most machinery bolting: M8 at 8.4/9.0/10 mm, M10 at 10.5/11/12 mm, M12 at 13/13.5/14.5 mm. Note the medium clearances grow slightly faster than the bolts — 9.0 is +1.0 over M8, 13.0 is +1.0 over M12, 11 is +1.0 over M10 — and that the M12 close hole (13 mm) equals the M12 nominal plus a full millimeter. If a design keeps wanting the coarse column at these sizes, the position tolerances upstream are the actual problem.
13/64″ for #10, 17/64″ for 1/4, 21/64″ for 5/16, 25/64″ for 3/8 — each one drill size over nominal, each fitting both the coarse UNC and fine UNF pitch of its size. The 13/64 #10 hole is worth memorizing: it is the most-asked clearance drill in imperial land, and it works for 10-24 and 10-32 alike.
M16 at 17/17.5/18.5 mm and M20 at 21/22/24 mm are structural-steel territory, where holes get punched, drilled with magnetic presses, or flame-cut. At these diameters the hole-to-hole position on the pattern matters more than the fit column — which is where the bolt circle coordinate methods earn their keep before any drilling starts.
The size-specific and standards questions this chart gets asked most — answered from ISO 273 and ASME B18.2.8.
A bolt hole tolerance calculator gives you the minimum hole; what happens around it decides whether the joint holds. Once the clearance hole chart has set your hole and the bolt circle layout has set your pattern, size the fastener itself with the free bolt torque calculator — same standard-first approach, covering preload, strength check, and the min/max assembly range. The bolt calculators hub also covers shear, length, weight, and concrete anchoring, so hole, bolt, and torque decisions all come from one consistent reference.
Hole sizing never travels alone — these companions cover the rest of the joint.
Weigh a complete fastener set: hex bolt plus nut and washer options, per-piece and total weight by quantity. Free, instant, no sign-up.
Check bolt shear stress with interactive sliders: bolt count, diameter, single or double shear, grade-based allowable stress and pass/fail safety check.
Get X/Y hole coordinates from a bolt circle: BCD from chord or across-holes measurements, hole angles, uneven spacing — flanges, wheels, chainrings.
Work out bolt length from grip, nut height and protrusion: through-bolt, A325 structural, TC bolt and flange stud scenarios, rounded to standard sizes.
Estimate concrete anchor capacity: breakout tension from embedment, F1554 rod strength, projection above the slab and J-bolt weights — ACI 318 style.
Metric and SAE bolt torque spec charts: Class 8.8/10.9/12.9 and Grade 5/8 values dry and lubricated, plus B7 stud, B8 stainless and SHCS rows.
Hex head and hex nut dimensions for M5–M30 and 1/4–1 inch sizes: across flats, head height, nut thickness, heavy hex and SAE–metric conversion.