How to Read GD&T on a Machined Part Drawing

Geometric dimensioning and tolerancing (GD&T) defines the allowable variation in a part's geometry as tolerance zones tied to the surfaces that matter in the assembly. In the United States the governing standard is ASME Y14.5, currently the 2018 edition; drawings from Europe and Asia more often follow ISO 1101 and the related ISO GPS standards. The symbols mostly look the same but some default rules differ, so the first thing to read on any drawing is the note stating which standard and edition apply.

Feature control frame anatomy

A feature control frame is the rectangular box attached to a feature by a leader or placed under a size dimension. It reads left to right:

1. Geometric characteristic symbol. What is being controlled: flatness, position, profile and so on.
2. Tolerance zone. A diameter symbol if the zone is cylindrical, then the tolerance value, which is the total width or diameter of the zone.
3. Modifiers. Material condition (a circled M or L) and others such as projected zone or free state.
4. Datum references. Primary, secondary and tertiary, in separate compartments.

Take a frame containing the position symbol, Ø0.005" (0.127 mm) with a circled M, and the datum letters A, B and C. It says that the axis of the feature must lie within a cylindrical zone of that diameter when the feature is at maximum material condition, and that the zone is located by basic dimensions from a datum reference frame established on A, then B, then C.

Basic dimensions, shown in a rectangular box, give the theoretically exact location or shape. They carry no tolerance; the tolerance is in the feature control frame.

Datums and the datum reference frame

A datum feature is a real surface on the part: a face, a bore, a slot. A datum is the theoretically exact plane, axis or point derived from it. The datum reference frame is the set of three mutually perpendicular planes built from the datums, and it is the coordinate system in which all related tolerances are measured.

A free part has six degrees of freedom, three translations and three rotations. For the common case of three planar datum features:

• The primary datum contacts the part on at least three points and removes three degrees of freedom: one translation and two rotations.
• The secondary datum contacts on at least two points and removes two more: one translation and one rotation.
• The tertiary datum contacts on at least one point and removes the last translation.

Order matters. Swapping primary and secondary changes how the part sits and therefore changes every measured result. A cylindrical primary datum such as a bore or journal behaves differently: its axis constrains two translations and two rotations.

Tip: Choose datum features the way the part is assembled. The face that bolts to the mating part is the primary datum; the pilot bore or dowel holes that locate it are secondary and tertiary.

The five characteristic families

ASME Y14.5-2018 defines twelve geometric characteristics in five families. Concentricity and symmetry, present in earlier revisions, were removed in 2018 in favor of position, runout and profile. ISO 1101 retains them.

Table 1. Characteristic families, what they control and how they are typically measured

Controls nest. An orientation tolerance applied to a surface also limits its form: a face held parallel within 0.002" (0.05 mm) cannot be less flat than that, so a separate flatness callout is needed only if it is tighter. Position controls the location and orientation of an axis or center plane, not the form of the surface. Profile of a surface is the most general control. With a full datum reference frame it controls size, form, orientation and location at once, which suits contoured surfaces defined by a CAD model.

Under ASME Y14.5, the size tolerance of a regular feature of size also controls its form: at maximum material condition the feature must have perfect form (Rule #1, the envelope principle). ISO drawings do not assume this by default.

Position versus coordinate tolerancing

Locating a hole with ±0.005" (±0.127 mm) in X and Y creates a square tolerance zone 0.010" (0.254 mm) on a side. The hole center may be off by 0.005" (0.127 mm) along an axis but by 0.007" (0.18 mm) toward a corner of the square. A bolt in a clearance hole is indifferent to direction, so the square zone accepts on the diagonal an error that it rejects along an axis.

A position tolerance with a diameter symbol creates a cylindrical zone. A Ø0.014" (0.36 mm) zone circumscribes that same square and has about 57% more area (the area ratio of a circle to its inscribed square is π/2). It allows nothing worse than the coordinate tolerance already allowed at its corners. Position also states which datums the location is measured from and in what order, which plus/minus dimensions leave ambiguous, and basic dimensions do not accumulate tolerance along a chain.

Position error is reported as a diameter: twice the radial distance from the true position to the measured axis. The guide to reading a CMM inspection report shows how that appears in inspection data.

Material condition modifiers and bonus tolerance

Material condition modifiers apply only to features of size such as holes, pins, slots and tabs:

• Maximum material condition (MMC). The most material: the smallest hole, the largest pin.
• Least material condition (LMC). The least material: the largest hole, the smallest pin.
• Regardless of feature size (RFS). The default when no modifier is shown. The stated tolerance applies whatever the feature's size.

With an MMC modifier, the stated tolerance applies when the feature is at MMC and grows as the feature departs from it. That growth is the bonus tolerance. Take a hole of Ø0.250"–0.255" (6.35–6.48 mm) with a position tolerance of Ø0.005" (0.127 mm) at MMC. A hole produced at Ø0.253" (6.43 mm) has departed from MMC by 0.003" (0.076 mm), so its allowable position error is Ø0.008" (0.203 mm). The worst-case boundary the mating pin sees, the virtual condition, stays constant at Ø0.245" (6.22 mm), which is why MMC callouts can be checked with a fixed functional gauge.

Use MMC where the function is clearance assembly, such as bolt patterns. Use RFS where location matters independent of size: press fits, alignment features, rotating parts. LMC protects a minimum wall thickness or edge distance.

Callouts that inflate cost

Over-tolerancing. Tight values copied from an earlier drawing or applied through a title block cost money on every feature they touch. Cost does not rise in proportion as a tolerance tightens. At some point the tolerance forces an extra operation such as grinding or honing, slower cutting, temperature control or full inspection. Every callout also becomes a line item in a first article inspection, so it carries an inspection cost as well as a machining cost.

Datums on non-functional features. A datum placed on a convenient outside edge instead of the mounting face means the part is inspected in a way it never sits in service. Small or short datum features are also unstable, because a slight error in a short datum surface is magnified over a long part.

Unmeasurable callouts. Examples are a datum symbol attached to a centerline instead of a physical feature, a position tolerance with no basic dimensions, and tolerances tighter than the available measurement uncertainty can resolve.

Common mistake: Applying one tight general profile or position tolerance to the whole model. Every feature then has to be machined and inspected to a value that only a few of them need.

Checklist

• State the governing standard and revision in the drawing notes.
• Confirm every datum feature is a physical, accessible surface that locates the part in its assembly.
• Check that located features have basic dimensions back to datums referenced in functional order.
• Review each tolerance tighter than the general tolerance and record why it is needed.
• Establish how each callout will be measured, by CMM metrology, a gauge or hand tools, before release.