Engineering Tolerances,
Fits and GD&T —
A Practical Guide

Dimensional tolerances and geometric tolerances are the language by which a mechanical engineering drawing communicates the acceptable variation in a manufactured part. Without them, a drawing defines a single perfect geometry that cannot be manufactured; with them, it defines a range of geometries that will function correctly when assembled and in service. Specifying tolerances correctly — tight enough to ensure function, generous enough to be manufacturable at reasonable cost — is a fundamental design skill. Specifying them incorrectly produces parts that either cannot be assembled or are unnecessarily expensive to make.

This article covers the ISO 286 system of dimensional tolerances and fits, the selection of hole-basis and shaft-basis fits for different assembly types, and the fundamentals of geometric dimensioning and tolerancing (GD&T) under ISO 1101 and ASME Y14.5.

The ISO 286 System — Dimensional Tolerances

ISO 286 defines a standardised system of tolerances for cylindrical features (holes and shafts) based on two parameters: the tolerance grade and the fundamental deviation.

The tolerance grade (IT grade, from IT01 to IT18) defines the size of the tolerance zone — the difference between the maximum and minimum permitted dimension. IT01 through IT4 are for high-precision gauge manufacture; IT5 through IT10 cover precision machined parts; IT11 through IT14 are for general machining; IT15 and above are for rough processes such as casting and forging. For each nominal size range, the tolerance value for each IT grade is tabulated in ISO 286-1.

The fundamental deviation (defined by a letter — uppercase for holes, lowercase for shafts) defines the position of the tolerance zone relative to the nominal dimension. The deviation establishes whether the tolerance zone sits above or below the nominal size and by how much. Letters A through H (holes) and a through h (shafts) are below (or touching) the nominal, creating clearance fits when paired; letters K through ZC (holes) and k through zc (shafts) are above (or touching) the nominal, producing interference or transition fits. The letter H (zero deviation for holes) and h (zero deviation for shafts) are the standard reference: an H hole has its lower limit at the nominal dimension; an h shaft has its upper limit at the nominal dimension.

Hole Basis vs Shaft Basis Fits

The majority of engineering fits use the hole basis system — the hole is held at a standard H tolerance grade and the shaft tolerance is varied to produce the required fit. This is preferred because holes are harder to machine to a precise deviation than shafts; broaches, reamers, and boring tools produce H-basis holes naturally, and it is easier to adjust the shaft diameter by turning or grinding than to adjust hole diameter precisely.

In the shaft basis system, the shaft is held at a standard h tolerance and the hole is varied. This is used where the shaft is a standard item (a bought-in shaft, a key, or a ground bar stock) that cannot be altered, and the housing must be machined to suit it.

Fit Types — Clearance, Transition, Interference

General Tolerances — ISO 2768

Not every dimension on a drawing needs an explicitly stated tolerance. ISO 2768 defines general tolerances that apply to all dimensions on a drawing that do not carry individual tolerances. ISO 2768-1 covers linear and angular dimensions in four classes (f, m, c, v — fine to very coarse); ISO 2768-2 covers geometric tolerances for features without individual geometric tolerances, in three classes (H, K, L). The applicable class is stated in the title block as, for example, "General tolerances to ISO 2768-mK." This approach reduces drawing clutter and communicates the overall manufacturing quality level required without explicitly tolerancing every feature.

Geometric Dimensioning and Tolerancing — GD&T

Dimensional tolerances (±X.XX) control size and location of features in a Cartesian sense. GD&T (ISO 1101 / ASME Y14.5) extends this to control the shape, orientation, and position of geometric features in a way that more precisely defines function and allows more intelligent interpretation by manufacturing. GD&T uses standardised symbols placed in feature control frames on the drawing.

Form Tolerances — No Datum Required

Form tolerances control the shape of individual features and do not require a datum reference:

• Flatness ⏥ — the entire surface must lie between two parallel planes separated by the tolerance value. Used on faces of flanges, seating surfaces, and mating faces where surface contact is critical.
• Straightness ⏤ — can apply to a line element on a surface (surface must lie within two parallel lines in that cross-section) or to a derived median line (the axis of a cylinder must lie within a cylindrical tolerance zone of the specified diameter).
• Roundness ○ — the cross-section of a cylindrical or conical feature must lie within two concentric circles separated by the tolerance value. Applied to each cross-section independently — does not control taper or straightness.
• Cylindricity ⌭ — the surface of a cylinder must lie within two coaxial cylinders separated by the tolerance value. Controls roundness, straightness, and taper simultaneously — the complete form of a cylindrical surface.

Orientation Tolerances — Datum Required

• Perpendicularity ⊥ — the feature must lie within a tolerance zone that is exactly perpendicular to the datum. Applied to faces and axes of threaded holes, bored holes, and mating surfaces.
• Parallelism ∥ — the feature must lie within a tolerance zone parallel to the datum.
• Angularity ∠ — the feature must lie within a tolerance zone at the specified angle to the datum.

Location Tolerances — Datum Required

• Position ⊕ — the most widely used GD&T symbol. Controls the location of a feature (typically a hole axis) relative to a datum reference frame. The position tolerance defines a cylindrical zone (diameter stated with ∅ modifier) within which the actual hole axis must lie. Unlike ± coordinate tolerancing, position tolerance with the ∅ modifier gives 57% more tolerance area for the same worst-case constraint, which means more parts pass inspection without compromising assembly function.
• Concentricity and Coaxiality ◎ — the derived median points (concentricity) or axis (coaxiality) of the controlled feature must lie within a cylindrical tolerance zone coaxial with the datum axis. Applied to rotating features where dynamic balance requires true concentricity rather than just size control.
• Symmetry ≡ — the derived median plane of the controlled feature must lie within two parallel planes symmetrical about the datum.

Runout Tolerances

• Circular runout ↗ — when the part is rotated about the datum axis, each cross-sectional element of the surface must lie within a tolerance band of the specified width in each measuring plane. Controls out-of-roundness and wobble combined for each cross-section.
• Total runout ↗↗ — the entire surface must lie within a tolerance cylinder coaxial with the datum axis when the part is rotated. Controls total surface variation — the tightest runout requirement.

Datum Reference Frames

GD&T orientation and location tolerances reference datum features — surfaces, axes or points on the part that establish the coordinate frame from which controlled features are measured. Datums are selected to reflect how the part is located in assembly: the primary datum (A) removes three degrees of freedom (typically the main mounting face), the secondary datum (B) removes two more (typically a bore or edge), and the tertiary datum (C) removes the final degree of freedom. Datum selection that reflects the assembly function ensures that parts which pass inspection will assemble correctly in practice, and that parts which fail inspection would genuinely not function — neither over-inspection nor under-inspection.

Surface Finish and Tolerances Together

Dimensional and geometric tolerances define where material must be; surface finish (Ra or Rz) defines the texture of that material. The two interact: a flatness tolerance of 0.01 mm is meaningless on a surface with Ra 3.2 μm (grinding marks 6–8 μm peak-to-valley), because the surface roughness itself will exceed the flatness tolerance. For tight geometric tolerances, surface finish must be specified compatible with the tolerance value — typically Ra ≤ tolerance value / 4 as a working rule.

Summary

The ISO 286 tolerance system provides a standardised framework for dimensioning holes and shafts, with tolerance grade (IT number) controlling the size of the tolerance zone and fundamental deviation (letter) controlling its position relative to nominal. H7/h6 and related hole-basis fits are the standard vocabulary for precision location and running fits. GD&T under ISO 1101 or ASME Y14.5 extends control to geometric form, orientation and position, allowing drawings to communicate functional requirements more precisely and economically than ± coordinate tolerancing alone. The position symbol with diameter modifier is the most important GD&T tool for bolt circles and hole patterns. Datums are chosen to reflect assembly function, not manufacturing convenience.