ISO 286 defines a system of tolerances for holes and shafts that establishes how precisely a cylindrical feature must be made and where its tolerance range falls relative to the nominal (design) dimension. The designation combines a letter (which indicates the position of the tolerance relative to nominal) and a number (which indicates the size of the tolerance band).
For holes, capital letters are used. "H" is the most common designation for holes in engineering drawings — it means the lower limit of the hole size is exactly at the nominal dimension. An H7 ½" hole must be at least 0.500" diameter; the upper limit depends on the number (7) and the nominal size. This ensures that an H-class hole is always at or above nominal — never undersize.
For shafts, lowercase letters are used. A shaft designated "p6" would be an interference fit shaft; an "e8" would be a clearance fit shaft. When you see a drawing callout like "25H7/p6", that's a 25mm bore with H7 tolerance paired with a p6 shaft — typically a press fit.
The number after the letter indicates the tolerance grade — IT grade (International Tolerance grade). IT grades run from IT1 (tightest, micron-level) to IT18 (loosest). For machined features:
IT5–IT6: Very precise. Precision grinding, honing, or fine reaming. Required for precision bearings, measurement instruments, and high-accuracy shaft/bore fits.
IT7: Precision reaming territory. The standard for interference fits, close clearance fits, and gear/bearing bores. Achievable with careful reaming in a well-maintained machine. H7 is the most commonly specified tolerance for precision bored holes in engineering.
IT8: Good quality reaming or careful boring. More tolerance than H7, appropriate for sliding clearance fits where some play is acceptable. H8 is achievable with less setup precision than H7.
IT9–IT11: Drilling range. H11 in particular is achievable with a good quality twist drill in a rigid setup. It's used for clearance holes (fastener through-holes, linkage pivot points with loose clearance).
IT12–IT14: Stamping, casting, non-precision machining. Holes you don't measure but just use for bolt clearance or non-critical fit.
H7 is the tolerance you'll see most often on precision engineering drawings for bore features that have a fit requirement. What does H7 actually mean in practical sizes?
For a 0.500" (12.7mm) nominal bore: H7 tolerance is +0.0007"/+0.0000" → acceptable range is 0.5000" to 0.5007". That's a 0.0007" total band with the lower limit at nominal.
For a 25mm nominal bore: H7 is +0.021mm/+0.000mm → 25.000mm to 25.021mm.
To hit H7 consistently, you need:
A pre-drilled hole close to correct diameter (within 0.010"–0.015" of nominal, see ream allowance). A quality machine reamer in good condition. A rigid setup with the reamer running true — any runout in the spindle or chuck adds to hole diameter and can push you outside tolerance. Consistent cutting speed and feed — H7 requires process discipline, not just good tooling.
H7 is not achievable with a twist drill alone in most shop conditions. It requires reaming.
H8 has a wider tolerance band than H7. For 0.500" nominal, H8 is approximately +0.0012"/+0.0000" → 0.5000" to 0.5012". That's nearly double the tolerance band of H7.
H8 is achievable with careful reaming but also with high-quality boring in a well-maintained machine. It's the right choice when a shaft needs to slide in a bore with controlled clearance — a sliding clearance fit — rather than the tight clearance of a precision bearing bore.
Many shops can hit H8 with a good quality reamer on a drill press or mill, where H7 would require a dedicated reaming cell or a more controlled process.
H11 has a much wider tolerance band. For 0.500" nominal, H11 is approximately +0.003"/+0.0000" → 0.5000" to 0.5030". That's 3 mils of total allowable variation.
H11 is used for clearance holes — the holes you drill for bolts, screws, and fasteners where the fastener passes through and the fit doesn't matter beyond "bolt goes through hole, doesn't fall out." It's also used for loose pivot and hinge applications where exact clearance isn't critical.
A quality twist drill in a rigid setup can hit H11 consistently. You don't need reaming, boring, or process control beyond normal drilling practice to meet this tolerance class.
If the drawing says H7: Plan for drilling + reaming. Size the pre-drill appropriately (nominal minus 0.010"–0.015" for most materials), use a precision machine reamer, ensure your setup is rigid and the reamer runs true. Verify with a plug gauge or calibrated bore gauge — don't assume the drill and reamer combination hits H7 without measurement the first time through.
If the drawing says H8: Reaming is still the right approach but with less process control required. A good quality reamer in a manual mill setup can produce H8 reliably with care. Verify dimensions on new setups.
If the drawing says H9, H10, or H11: Drilling is your process. Choose drill size carefully — a sharp H11 drill will likely produce a hole that's 0.001"–0.003" oversize relative to its nominal diameter in most conditions. For H11, a drill at nominal diameter or slightly under is appropriate.
If no tolerance is called out: Most shops default to H11 or equivalent for through-holes with no callout. If the drawing has a general tolerance block, the tolerances there govern. When in doubt, ask the engineer or verify against the mating part.
The fit tolerance on a drawing tells you what process to use. H7 means reaming, which means you need a sharp pre-ream drill — and the pre-ream drill must be both the right diameter (to leave correct ream allowance) and producing a round, clean hole (so the reamer is cleaning up a good hole, not a wandered or torn one).
A dull pre-ream drill produces an out-of-round hole with work-hardened surfaces in some materials. The reamer then has to deal with irregular stock removal — cutting more on one side than the other — and the resulting reamed hole may be within diameter tolerance but out-of-round or with a poor finish. For H7 fit applications, pre-ream drill condition matters as much as the reamer condition.
A dull pre-ream drill produces a bore the reamer can't fully clean up. Keep your pre-ream HSS drills sharp — mail them in and we'll restore them to cutting geometry on the WinsloMatic.
Get a Quote →