How to Identify Missing Dimensions in an Engineering Drawing

What a fully defined drawing means

Both major drawing systems start from the same principle. ASME Y14.5-2018 sets out fundamental rules that, in short, require every dimension to carry a tolerance (reference, maximum or minimum, and stock dimensions aside), require the dimensioning to be complete enough that each feature is fully understood, and do not permit sizes to be measured from the drawing or assumed. ISO 129-1 states the same principle of complete dimensioning for ISO drawings, with each feature dimensioned only once.

A useful way to think about completeness comes from CAD itself. A sketch is fully constrained when nothing in it can move. A drawing is fully defined, in the same sense, when every feature has a size and a position (and an orientation, where it matters) fixed by something the drawing states, and when each of those values has a tolerance. A missing dimension is a degree of freedom the drawing leaves open.

Missing dimension

A size, location or orientation of the part that cannot be determined from the drawing’s dimensions, notes, general tolerance, or the conventions of its stated standard, without measuring the drawing or assuming a value.

Stated, implied, derived and missing

Not every value has to appear as a number next to the feature. Sort each value you need into one of five groups.

The centerline case

A hole drawn on the centerline of a plate, with no location dimension, is the most common judgment call. By convention it is centered. Whether that is complete depends on how the drawing controls location. Under ASME Y14.5, where such a feature is located with GD&T, its distance from the centerline it is drawn on is generally read as an implied basic zero, and the positional tolerance governs. On a drawing without GD&T, the nominal location is clear but the allowed variation often is not stated anywhere. Treat the location as defined at nominal and raise the tolerance as a question unless the drawing answers it.

Reference dimensions are not definitions

A reference dimension is shown in parentheses, on ASME and on ISO drawings (ISO 129-1 calls it an auxiliary dimension). It is information, usually a value that can be derived from other dimensions, and it carries no tolerance. Nobody inspects to it. Two checks follow. First, a reference dimension should duplicate something the drawing already defines: if the only place a size appears is in parentheses, the feature is not properly defined, even though you could model its nominal value. Second, a reference dimension that disagrees with the dimensions it repeats points to an error in one of them.

General tolerance blocks

A dimension shown without its own tolerance takes the drawing’s general tolerance. On ISO drawings that is often an ISO 2768-1 class: f (fine), m (medium), c (coarse) or v (very coarse), noted in the title block, for example as ISO 2768-m. Its permitted deviations depend on the size range of the dimension, so look the value up in the standard rather than from memory. On ASME-style drawings, the title block often gives tolerances by the number of decimal places shown.

• No general tolerance anywhere. Every untoleranced dimension is then incomplete. This is a gap even if every nominal value is present.
• Two general tolerances. A title-block table and a note that disagree. Ask which governs.
• Angles. Check that the general tolerance covers angular dimensions too, including the implied right angles.
• Decimal-place tables. A table keyed to decimal places reads differently when a value is written as 12 or as 12.0; make sure the drawing’s practice is consistent.

Fits are a related check. A tolerance class such as Ø20 H7 is complete only with its fundamental deviation letter and grade, per ISO 286-1. The limit dimensions tool turns a nominal size and its deviations into limits, and the fit calculator gives the clearance or interference from hole and shaft limits you enter; the deviations for a designation come from ISO 286-2.

Dimension chains and closure

Chain dimensioning locates each feature from the previous one; baseline dimensioning locates each from a common datum. Chains have two failure modes, and both are found by adding them up.

• An open chain. Take a plate 80 long with holes located 10, then 30, then 30 from its left edge. The last segment, 10 to the right edge, is derivable (80 − 10 − 30 − 30). The geometry is defined, but the right-hand edge distance carries the accumulated tolerance of four dimensions. Check whether that is acceptable for its function.
• A closed chain. The same plate with all four segments and the overall length dimensioned, all toleranced. The part is now over-defined: the segments and the overall cannot all be held at their limits at once. One of them should be a reference dimension. This is not a missing dimension, but it belongs on the same question list.
• A chain that does not add up. If the segments sum to 79 against an overall of 80, one value is wrong. Never decide which one.

The tolerance stack-up tool works out the worst-case and statistical variation of a chain once it is complete.

Hole patterns

Patterns deserve their own pass, because the callout carries the count and size and it is easy to assume the rest.

• Count. The callout’s count (6X) matches the instances drawn.
• Size and depth. Diameter, THRU or a depth, and any counterbore or countersink with its own diameter and depth or angle.
• Spacing in both directions. A rectangular pattern needs a pitch in X and in Y.
• Pattern location. Where the pattern sits relative to the datums: often its center or its first hole. A pattern with spacing and no location floats.
• Bolt circles. The pitch-circle diameter, the angular spacing (or an equal-spacing note), and the clocking: the angle of the first hole from a datum. Clocking is easy to leave out.
• Threads. A complete designation (size, and pitch where it is not the coarse default; for ISO metric threads an omitted tolerance class means the medium class, 6H or 6g from M1.6, per ISO 965-1), and for blind holes the thread depth, with the drill depth where the design needs it.

A practical checklist

Write the gap as a question

Write each gap as one question that names the feature, its place on the sheet and what is missing; the ambiguity guide covers how to word it, how to record the answer, and when the work must stop.