Guide
What H7 hole tolerance can a drilled hole hold, and when does it need a reamer or boring?
H7 hole tolerance is the ISO 286 tolerance class that puts the smallest allowed hole exactly at the nominal size and lets it grow by one IT7 band, the standard grade for dowel holes, bearing seats and locating bores. A plain twist-drilled hole almost never holds it reliably, so an H7 callout is really a process decision: drill and ream, or drill and bore.
By Saola Manufacturing engineering team · Published · Updated
This guide is about the hole, not the fit. It shows what an H7 band is in micrometers and inches, what a drilled hole actually delivers, how to choose between a reamer and a boring tool, and how to write the callout and the RFQ so the supplier quotes the right route. For the interference and clearance a given pin or shaft produces in that hole, see the separate guides on clearance, transition and interference fits and press fits for dowel pins and bearings. Values quoted below are from the standards or are labeled as typical practice; they are not the capability of any particular shop.
On this page
How wide is an H7 hole tolerance at common sizes?
Per ISO 286-2, an H7 hole has a lower deviation of zero and an upper deviation equal to the IT7 grade for its size, so a 10 mm H7 hole may measure anywhere from 10.000 to 10.015 mm. The band widens with diameter, which is why an H7 callout is never a single number.
The letter H fixes where the band starts: at nominal, never below it. That is what makes a hole-basis system work, because a standard pin, gauge or reamer can be made to one known minimum. The number 7 fixes how wide the band is, and ISO 286-1 scales that width with size, so the same grade represents roughly the same level of difficulty on a small hole and a large one. The US metric fits standard, ASME B4.2, uses the same hole-basis classes (ASME B4.2).
The comparison columns matter more than the H7 column itself. IT9 is roughly where general-purpose machining sits and IT11 is typical of a plain drilled hole, and both are several times wider. When a drawing moves a hole from an IT11-type tolerance to H7, it is not tightening it a little; per ISO 286-1 it is asking for a band roughly one sixth as wide, and that almost always adds an operation.
| Nominal size (mm) | H7 limits (µm) | H7 band (in) | IT9 band (µm) | IT11 band (µm) |
|---|---|---|---|---|
| over 3 up to 6 | 0 to +12 | 0.00047 | 30 | 75 |
| over 6 up to 10 | 0 to +15 | 0.00059 | 36 | 90 |
| over 10 up to 18 | 0 to +18 | 0.00071 | 43 | 110 |
| over 18 up to 30 | 0 to +21 | 0.00083 | 52 | 130 |
| over 30 up to 50 | 0 to +25 | 0.00098 | 62 | 160 |
| over 50 up to 80 | 0 to +30 | 0.00118 | 74 | 190 |
What tolerance does a plain drilled hole actually hold?
As typical industry guidance, a hole from a standard twist drill lands somewhere in the IT10 to IT13 range and usually comes out slightly larger than the drill. A modern solid-carbide drill with through-tool coolant does noticeably better, but it is still generally treated as a grade or two short of a dependable H7.
Size is only one of the problems. A twist drill has two cutting lips and is guided only by its own margins once it is in the cut, so the hole it makes tends to be slightly out of round, often with a three-lobed shape, a little bell-mouthed at the entry and, on deep holes, drifting off its axis. Surface texture is coarse compared with a reamed or bored wall. Twist drill nomenclature, sizes and tolerances are set by the drill standard (ASME B94.11M, Twist Drills), but those limits apply to the tool, not to the hole it produces; runout in the spindle, point grinding, material and coolant all add to the result.
That makes the practical rule simple. If the hole only has to pass a bolt, a pin with clearance, a cable or a coolant passage, leave it drilled and give it a tolerance that matches drilling. If the hole has to locate something, carry a dowel, seat a bearing or guide a sliding pin, it needs a finishing operation, and H7 is the normal way to say so. Putting H7 on a bolt clearance hole is one of the most common ways a drawing adds cost for no function; the guide to the cost of tight tolerances covers how that adds up across a whole part.
When is reaming the right way to finish an H7 hole?
Reaming is the right choice when the hole is a standard diameter, small to medium in size, already in the right place, and needs good size, roundness and finish quickly and repeatably. A reamer corrects size and roundness, but it follows the pre-drilled hole, so it does not correct position or straightness.
As typical catalog practice, stock metric machine reamers are ground to cut an H7 hole at standard diameters; reamer types and nomenclature are covered by their own tool standard (ASME B94.2, Reamers). Because the reamer is a fixed-size tool, every hole in a batch is cut by the same diameter, which is why reaming is so repeatable once the first parts are proven. It is also fast: one pass, no adjustment between parts.
Three conditions decide whether reaming works in practice:
- Stock allowance. The pre-drilled hole has to leave the reamer the right amount to cut. As typical industry guidance for machine reaming, that is a few tenths of a millimeter on diameter for small and medium holes. Too little and the reamer rubs and burnishes, leaving an undersize, glazed hole; too much and it chatters or cuts oversize.
- Position comes from the drill. A reamer floats along the existing hole. If a dowel hole has a tight position tolerance, the drilled hole must already be in position, typically by spot drilling first, keeping drills short and rigid, or by finishing the hole with a boring tool instead.
- Material behavior. Some materials close up after the reamer leaves, others cut slightly oversize. Aluminum, stainless steel and cast iron all behave differently, so the first-article measurement, not the reamer marking, decides whether the tool is right for the job.
Blind holes need extra thought. A reamer has a lead chamfer at its tip, so the last part of a blind hole is not full diameter. The drawing should give the depth of full-diameter H7 wall that is actually needed, and the drill depth should be allowed to run deeper to leave room for the chamfer and for chips.
When should an H7 hole be bored instead of reamed?
Bore the hole when its position, straightness or perpendicularity matters as much as its size, when the diameter is large or non-standard, or when the hole starts as a cast or cored opening. A boring tool is a single-point cutter set to size, so it cuts its own axis instead of following the one it finds.
The usual triggers for boring are:
- Bearing seats and large bores. Above the sizes where stock reamers are economical, an adjustable boring head or boring bar is the normal finishing tool.
- Holes that must be on location. A locating bore tied to a datum with a tight position or perpendicularity tolerance should be bored, because boring corrects the drift that a drill introduced.
- Cast and cored holes. A core in a die casting can shift slightly, and a reamer would follow that shifted hole. A boring operation brings it back to the machined datums; the guide to die-casting machining allowance covers how much stock to leave on a cored bore.
- Odd diameters. A hole that falls between standard reamer sizes needs either a special reamer or a boring tool, and for modest volumes the boring tool usually wins.
The cost of boring is time and attention: the tool has to be set, often adjusted in small steps, and checked as it wears, so it is slower per hole than reaming. Helical interpolation with an end mill is a third route for larger holes, but as typical industry guidance it is not relied on to hold IT7 batch after batch, so on an H7 feature it is usually a roughing or semi-finishing step before a bore or reamer.
How should an H7 hole be called out on the drawing and the RFQ?
Call out the result you need, the class, the full-diameter depth, the finish and the position relative to datums, and let the supplier choose the route. Add the actual limits in brackets so that nobody has to look them up.
Writing “REAM” on a drawing is tempting, but ASME Y14.5 treats the drawing as a description of the finished part, not of the process (ASME Y14.5). If the hole is specified completely, a supplier can ream it, bore it or grind it and the part still conforms. If the process is written instead of the requirement, a hole that was reamed but is out of position technically meets the note and still fails the assembly.
| Hole function | Example callout | What it tells the supplier |
|---|---|---|
| Dowel hole, blind | Ø8 H7 (8.000/8.015), 12 DEEP FULL DIA, Ra 1.6 | Finish operation needed; drill may go deeper |
| Dowel hole, on location | Ø8 H7 (8.000/8.015) THRU, position Ø0.02 to A|B|C | Position drives the route; likely bored or drilled on location before reaming |
| Bearing seat | Ø35 H7 (35.000/35.025), perpendicular 0.01 to A, Ra 0.8 | Bore, with in-process measurement |
| Bolt clearance hole | Ø9 THRU, general tolerance ISO 2768-m | Drill only; no H7 |
| H7 hole in an anodized part | Ø10 H7 (10.000/10.015) AFTER FINISH, or MASK | Finish allowance must be built into the machined size |
Two details on that list cause most of the arguments after first article. The first is whether H7 applies before or after plating or anodizing. A coating adds thickness to the wall and shrinks the hole, so a hole that was a good H7 when machined can gauge tight after finishing; the guide to anodizing dimensional change covers how much, and masking for anodizing covers the alternative of keeping the bore bare. The second is depth: on a blind dowel hole, say how deep the H7 wall must be, not just how deep the hole is.
On the RFQ itself, list each H7 hole by balloon number with its function (dowel, bearing, locating pin, sliding fit), the mating part’s tolerance class if known, any coating that covers the bore, and the inspection method you expect. That lets the supplier tell you up front which holes will be reamed, which will be bored, and whether any of them are tighter than what the process routinely holds.
How is an H7 hole inspected?
The standard production check is a plain GO/NO-GO plug gauge made to the H7 limits for that size, backed by a bore gauge or similar comparator when the actual size or the shape of the hole matters. Calipers are not a valid check for an H7 hole.
A GO plug the full length of the engagement proves that the hole is at least the minimum size along its length and is not bent or bell-mouthed enough to stop a pin, the same logic as the full-length GO member described in the guide to GO/NO-GO thread gauges. The NO-GO plug checks that the hole is not oversize where it is tried, usually at both ends of a through hole. What a pair of plugs cannot tell you is how close to a limit a hole sits, or whether it is out of round in a way that still lets a plug through, so a bore gauge is used on first article and wherever the drawing marks the hole as a controlled characteristic. A three-point bore gauge picks up the three-lobed shape a drill leaves, which a two-point gauge can read as round.
The measuring tool has to be much finer than the band it checks. Per ISO 286-2 the whole H7 band at 10 mm is 15 µm, while, as typical industry guidance, a digital caliper’s stated accuracy is about 20 µm, wider than the whole band, so a caliper reading inside the limits proves very little; the tight tolerance cost guide explains how measurement uncertainty shrinks the usable band. Temperature matters too: a hole measured warm, straight off the machine, reads differently from the same hole at the reference temperature, which per ISO 1 is 20 °C, so parts should be allowed to settle before they are checked.
How does Saola handle reamed and bored holes?
Reamed and bored holes are part of the secondary machining done on castings in the plant, and the milling page lists bores bored and reamed to print among its routine work. An H7 callout at most common sizes is tighter than the bore tolerance that page publishes, so flag every H7 hole on the RFQ.
The CNC milling page describes the work as the second operation after casting: datum faces machined flat, bores bored and reamed to print, tapped holes and pockets cut into aluminum and zinc die castings, and machined bores on sand-cast brass and bronze valve bodies. The same page asks designers to size bores to standard reamer and boring-bar diameters where the fit allows, because an in-between diameter forces a special tool or a slower cut, and to keep deep, tight-tolerance holes away from thin cast walls, where core shift can pull the hole off true. It also states plainly that the milling side is not a general billet-machining job shop and does not offer simultaneous five-axis work.
For bores in turned bar parts, flag H7 bores on the RFQ too, so they are reviewed feature by feature for CNC turning. The same page lists cross-drilled holes among the features cut routinely. The quality page describes a first-article inspection report that measures every toleranced dimension on the first piece from new tooling and a dimensional inspection record with each production lot. If a drawing carries H7 holes that are tighter than the published figures, the milling page asks for that to be raised before tooling rather than after first samples, so say so in the RFQ, or send the drawing for a quote and ask for a note on the proposed route for each hole.
Frequently asked
Can a drilled hole ever meet H7 without reaming?
Sometimes, on a given machine with a sharp carbide drill in a well-behaved material, a drilled hole will happen to measure inside H7. That is not the same as holding it batch after batch. Unless the supplier has shown capability data for that drill on that material, treat H7 as needing a finishing pass.
Is an H7 hole a press fit for a standard dowel pin?
Not reliably. A standard hardened dowel in an H7 hole gives a transition fit that can be slightly loose or slightly tight depending on where both parts land. If the pin must stay put, the hole class usually moves tighter; the press fit guide gives the numbers for each option.
What is the inch equivalent of H7?
There is no exact one. Inch drawings built on ANSI B4.1 use named classes such as LC and LT locational fits rather than letter-grade pairs, and their limits are not a unit conversion of ISO 286. If an inch drawing needs an H7-quality hole, write the limits in inches and, if helpful, add “equivalent to H7” as a reference note rather than mixing the two systems on one feature.
Does reaming fix a hole that was drilled in the wrong place?
No. A reamer follows the existing hole, so it improves size, roundness and finish but leaves the position and straightness where the drill put them. Position errors are corrected by boring, or prevented by spot drilling and using short, rigid drills.
Can an H7 hole be reamed in a die-cast part?
Yes, and it is common, but internal porosity can open up at the machined wall and a cored hole may have shifted. Leave enough stock to clean up, bore rather than ream when position matters, and read the guide to porosity after machining before specifying a sealing or bearing bore in a casting.
Sources
- ISO 286-1:2010, Geometrical product specifications (GPS), ISO code system for tolerances on linear sizes, Part 1: Basis of tolerances, deviations and fits, International Organization for Standardization, 2010
- ISO 286-2:2010, Part 2: Tables of standard tolerance classes and limit deviations for holes and shafts, International Organization for Standardization, 2010
- ISO 1:2022, Geometrical product specifications (GPS), Standard reference temperature for the specification of geometrical and dimensional properties, International Organization for Standardization, 2022
- ASME B4.2, Preferred Metric Limits and Fits, ASME, 1978 (R2020), standard page accessed 2026
- ASME B94.2, Reamers, ASME, 1995 (stabilized), standard page accessed 2026
- ASME B94.11M, Twist Drills, ASME, 1993, standard page accessed 2026
- ASME Y14.5, Dimensioning and Tolerancing, ASME, 2018 (R2024)