You've seen the callout on a drawing — 25 H7 or 12 H11 — and maybe you've written one yourself without being completely sure what those letters and numbers actually commit you to in manufacturing. Hole tolerance grades are one of the most consequential specifications a designer puts on a CNC part drawing, yet they're often applied by habit rather than intent. Choose too tight a grade and you inflate cost without gaining functional benefit. Choose too loose a grade and the assembly rattles, leaks, or fails to locate correctly.

This guide decodes the three most common hole tolerance grades used in CNC machined parts — H7, H8, and H11 — so you can apply them deliberately. We'll cover what the letters and numbers mean under ISO 286, the actual tolerance band values at common diameters, which shaft pairings work with each grade, and when to use each one. Whether you're designing a bearing housing, a sliding sleeve, or a loose clearance bracket, the right grade is a design decision — not a default.

What Is a Hole Tolerance Grade?

A hole tolerance grade is a standardized specification that defines how much a drilled or bored hole is allowed to deviate from its nominal (basic) size. Rather than writing an explicit bilateral tolerance like 25.000 +0.021/+0.000 mm on every feature, engineers use ISO 286 shorthand codes — such as H7, H8, or H11 — that convey the same information in two characters. The machinist, inspector, and supplier all interpret the code the same way, because ISO 286 maps every letter-number combination to precise upper and lower deviation values across a full range of nominal diameters.

The system is built around two components: a fundamental deviation (the letter) and a tolerance grade (the number). Together, they define where the tolerance zone sits relative to the nominal size and how wide that zone is. For holes, capital letters are used. The letter H is by far the most common hole designation in CNC work because it places the lower limit of the hole exactly at the nominal size — the hole can only be at or above nominal, never below it. This makes H-series holes straightforward to machine and inspect, and it's why they form the basis of the widely adopted hole-basis system.

How to Read the Code: Decoding H7, H8, and H11

Every ISO hole tolerance code follows the same structure: a capital letter followed by a number. The letter (in this case, always H) tells you the position of the tolerance zone. In the hole-basis system, H means the lower deviation is zero — the minimum acceptable hole size equals the nominal diameter exactly. The number represents the International Tolerance (IT) grade, which defines the width of the tolerance band. Lower numbers mean tighter tolerances; higher numbers allow more variation.

So in H7, the "H" fixes the bottom of the tolerance zone at nominal, and the "7" specifies IT grade 7 — a medium-precision band. In H11, the same zero-lower-deviation rule applies, but IT grade 11 is significantly wider, allowing more variation in the finished hole size. Because the lower limit is always zero for all H-series holes, the only variable between H7, H8, and H11 is the upper deviation — which increases as the grade number rises. This is the key insight: all three grades share the same starting point; what differs is how much bigger the hole is allowed to get.

When a fit is specified — for example, H7/g6 — the capital-letter portion describes the hole and the lowercase portion describes the mating shaft. The hole-basis system is the industry standard for most CNC applications because it is more economical: standard reamers and boring tools produce a fixed H-grade hole, and the shaft diameter is adjusted on a CNC lathe to achieve the required fit type.

H7 Tolerance: The Precision Workhorse

H7 is the most frequently specified hole tolerance grade in precision CNC machining, and for good reason. It provides a medium level of precision that suits the widest variety of functional applications — from bearing housings and locating features to sliding pins and guide bores — while remaining consistently achievable with standard boring, reaming, or finish milling operations. The tolerance band for H7 is defined by IT grade 7, which scales with nominal diameter. For a 25 mm hole, the H7 upper deviation is +0.021 mm (21 microns), meaning the hole must fall between 25.000 mm and 25.021 mm. For a 50 mm hole, the band widens slightly to +0.025 mm.

Because the H7 tolerance zone is relatively tight — typically ranging from approximately 10 to 40 microns across common diameter ranges — it requires controlled machining. Standard twist drilling alone rarely achieves it reliably; reaming, CNC boring, or finish passes on a machining center are the typical production methods. The surface finish of the bore also matters: a rough bore surface effectively reduces the functional clearance in a fitted assembly, so H7 holes are often specified with a corresponding surface finish requirement.

Common H7 shaft pairings and their applications:

• H7/g6 (Sliding fit): The most widely used precision clearance fit. The shaft is always slightly smaller than the hole, producing a clearance of approximately 0.007 to 0.041 mm at 25 mm diameter. Ideal for guide pins, precision slideways, shaft-in-bushing arrangements, and any feature where accurate location and free sliding movement are both required.
• H7/h6 (Locational clearance fit): Very close fit with minimal clearance — down to zero at the tightest end. Used for locating stationary parts that need to be assembled and disassembled by hand without force. Common in jig and fixture work and precision assemblies requiring repeatable re-location.
• H7/k6 (Transition fit): Depending on where each part falls within its tolerance band, the assembly may have a slight clearance or slight interference. Standard for rolling bearing inner ring seats under normal load conditions and for gear wheel hubs on shafts where a key or pin is also used.
• H7/p6 (Interference/press fit): The shaft is always larger than the hole, requiring force or thermal methods for assembly. Used for permanently fixed components such as press-fitted bearing outer races, gear hubs, and automotive wheel hub applications.

H7 is the right choice any time a part needs to locate accurately, rotate or slide with controlled clearance, or mate with a standard bearing. It is the baseline precision grade for CNC machining — neither over-engineered nor under-specified for the majority of functional mating features.

H8 Tolerance: The General-Purpose Grade

H8 sits one step looser than H7, using IT grade 8 to define a tolerance band that is roughly 60% wider at the same nominal diameter. For a 25 mm hole, the H8 upper deviation is +0.033 mm — compared to H7's +0.021 mm. That extra 12 microns of allowable variation doesn't sound significant, but it translates directly into a more forgiving machining process, fewer rejects, and lower unit cost, making H8 an excellent choice for general-purpose features where extreme precision is not functionally necessary.

H8 is most commonly paired with an f7 shaft to create a close running fit (H8/f7). At 25 mm diameter, this pairing produces a clearance range of approximately 0.020 to 0.074 mm — enough gap to support a consistent lubricating film between moving surfaces without the precision cost of an H7 hole. This makes H8/f7 well-suited to rotating shaft applications, piston-in-cylinder fits, sliding rods, and machine tool spindles where smooth, reliable motion matters more than tight alignment. Automotive pistons are a textbook example of this grade in use.

Common H8 shaft pairings and their applications:

• H8/f7 (Close running fit): The standard choice for rotating shafts in plain bearings and lubricated sliding assemblies. Good for moderate speeds and journal pressures. Applications include machine tool spindles, sliding rods, and regulator bearings.
• H8/h7 (Locational sliding fit): Very small clearance; parts can be assembled and disassembled without force and will slide freely once lubricated. Used for precise guiding and centering where some movement is acceptable.
• H8/js7 or H8/k7 (Transition variants): Occasionally used when a light transition fit is needed with the added manufacturing latitude of an H8 bore rather than H7.

For product designers working with components that need reliable movement but don't require the tightest possible alignment, H8 delivers meaningful cost savings. It is also a practical choice for plastic injection molded housings and die cast components that will receive a machined bore, since the slightly wider tolerance band is more compatible with the inherent dimensional variation of those processes. If your part is going through plastic injection molding or pressure die casting upstream, an H8 bore in a secondary machining operation often makes more practical sense than specifying H7.

H11 Tolerance: The Loose Clearance Grade

H11 is a coarse-grade tolerance class intended for applications where the hole does not need to locate or guide anything precisely — it just needs to clear. The IT grade 11 tolerance band is substantially wider than H7 or H8. For a 25 mm hole, the H11 upper deviation is +0.130 mm, giving a total tolerance band of 130 microns. That is roughly six times the band width of H7 at the same diameter. Standard CNC drilling can typically achieve H11 without a reaming pass, making it the most economical hole grade to produce.

The most common H11 fit pairing is H11/c11, which produces a loose running or free clearance fit. At 25 mm diameter, this combination gives a minimum clearance of approximately 0.110 mm and a maximum clearance of 0.370 mm. That amount of play is intentional — it accommodates misalignment, thermal expansion, contamination ingress, and rough assembly conditions. H11 holes appear in agricultural equipment, rough industrial machinery, pivots, latches, bracket mounting slots, and any application where the mating part needs to fit in without binding even under adverse conditions.

Where H11 is the right choice:

• Clearance holes for bolts and fasteners where no precision location is needed
• Slot and bracket features in sheet metal fabrication or structural assemblies
• Applications exposed to dirt, dust, corrosion, or heavy thermal cycling
• Pivot pins and latches where a loose, free-moving connection is the functional goal
• Draft fits on parts that need to assemble easily in field conditions without precision tooling

It is worth noting that H11 is not a "don't care" tolerance. It is a deliberate specification that communicates to the machinist and inspector exactly how much variation is acceptable. Calling out H11 explicitly is better practice than leaving a hole undimensioned and relying on a general tolerance block, because it makes the functional intent clear and connects the feature to a standard that inspection can verify consistently.

Comparing H7, H8, and H11 Side by Side

The table below summarizes the key differences between H7, H8, and H11 for a 25 mm nominal diameter, along with their typical applications and common shaft pairings. These values are derived from ISO 286-1.

The pattern is straightforward: as the IT grade number increases, the tolerance band widens, the fit becomes looser, the machining process becomes simpler, and the cost decreases. Most well-designed parts use a mix of all three grades — H7 on critical locating and bearing features, H8 on running-fit and secondary mating features, and H11 on clearance holes and non-critical through-holes.

How to Call Out Hole Tolerances on CNC Drawings

Applying an ISO hole tolerance to a CNC drawing is straightforward once you understand the notation. The standard format places the nominal diameter followed by the tolerance code directly: for example, Ø25 H7 or Ø12 H11. When the mating shaft is also being designed and its tolerance matters for fit prediction, the full fit designation is written as Ø25 H7/g6, with the hole tolerance before the slash and the shaft tolerance after it. Both parts are then machined to their respective grades, and the resulting clearance or interference falls within the range defined by ISO 286.

A few practical drawing conventions are worth keeping in mind. First, ISO hole tolerances apply to cylindrical features — bored holes, reamed holes, and precision-drilled holes. They are not typically applied to non-round features, slots, or external profiles, which use dimensional tolerances or GD&T callouts instead. Second, ISO 286 controls mating hole and shaft limits specifically; for undimensioned features elsewhere on the part, the general tolerance block (typically ISO 2768-m or ISO 2768-f) governs. Third, if a critical bore requires both a hole tolerance and a geometric control (such as cylindricity or position), both callouts should appear on the drawing — the ISO grade alone does not constrain form or location.

When working with a manufacturing partner like NICE Rapid, providing the full ISO fit designation on your drawing eliminates ambiguity during quoting, process planning, and inspection. It tells the machinist which tooling strategy is appropriate, tells the quality team what gauge to use, and tells the assembler what to expect. A clearly specified H7 bore on a CNC machined part is far less likely to generate a nonconformance than a bare nominal dimension with a generic ±0.05 mm block tolerance applied to a bearing seat.

The Tolerance-Cost Tradeoff: Why Grade Selection Matters

Tolerance grade selection is one of the most impactful Design for Manufacturability (DFM) decisions on a CNC part. Tighter tolerances require more controlled machining processes, additional tool passes, and more rigorous inspection — all of which add time and cost. The relationship is not linear: moving from H11 to H8 adds modest cost, but moving from H8 to H7 can require switching from a drilling operation to a reaming or boring operation, introducing a separate process step with its own setup time and tooling cost.

A useful mental model: H11 is achievable with standard CNC drilling in a single pass, making it the lowest-cost option. H8 typically requires a finish pass or a quality drill process with tight tool management. H7 generally demands reaming, precision boring, or careful CNC finishing with active measurement, and it may also require tighter temperature controls in the machining environment to avoid thermal growth affecting the bore. Only 10 to 20 percent of hole features on a typical well-optimized machined part actually need H7 or tighter. Applying H7 indiscriminately to every hole on a drawing is one of the most common ways designers unknowingly inflate part cost without improving function.

The right approach is to audit every hole on the drawing by function. Bearing seats, precision locating bores, and features that will be press-fitted all justify H7. Running fits and general mating features work well at H8. Clearance holes, bolt pass-throughs, and loose fit features should default to H11 unless there is a specific reason for tighter control. This intentional grade selection — rather than applying a single tolerance class across all holes — is the mark of an experienced designer and the fastest path to a cost-effective, manufacturable part.

Machining Hole Tolerances at NICE Rapid

At NICE Rapid, our CNC machining service is equipped to hold hole tolerances from loose clearance grades through precision H7 and tighter, across a wide range of materials including aluminum alloys, stainless steels, engineering plastics, and titanium. Whether you need a single prototype with a critical bearing bore or a production batch of housings with mixed tolerance requirements, our engineering team reviews drawings for tolerance achievability and manufacturability before cutting a single chip.

Our broader manufacturing capabilities also mean we can support your product across the full development lifecycle. Prototypes can begin as 3D printed or vacuum cast parts for early fit and form validation, then transition to CNC machined components as tolerances are refined and production volumes scale. If your design incorporates injection-molded or die-cast housings with machined bores, we manage both operations under one roof — ensuring that the H7 bore in the machined step is designed in context of the upstream casting or molding process. For sheet metal enclosures and brackets with clearance hole requirements, our sheet metal fabrication service applies the same tolerance discipline to every feature.

ISO certification and a global customer base across automotive, medical, consumer electronics, and industrial equipment sectors mean our quality systems are built to verify tolerance compliance rigorously — not just at the machine, but through documented inspection records that support your engineering sign-off. When you specify Ø25 H7 on your drawing and send it to NICE Rapid, that callout is understood, planned for, and verified — from quote through delivery.

Final Takeaway

H7, H8, and H11 are not interchangeable defaults — each is a precise specification that connects your design intent to a defined manufacturing process and a predictable assembly outcome. H7 delivers the precision needed for bearing seats, locating bores, and controlled fits. H8 provides an excellent balance of accuracy and cost for general running and sliding applications. H11 is the economical, practical choice for clearance holes and features where generous fit is the goal. Used deliberately, these three grades cover the vast majority of hole tolerance requirements on a CNC machined part, and specifying them correctly is one of the clearest signals to your manufacturing partner that your design is ready to produce.