GD&T fundamentals — AlpineTutor

Plus-minus dimensioning is fine for a length. It falls apart the moment you have to say where something is — and that is most of what a real drawing does.

Geometric Dimensioning and Tolerancing is the language that fixes it. It is harder to read and it makes parts cheaper, and this topic is about why both of those are true.

A precision machined steel plate with several closely spaced bored holes standing on a granite surface plate in an inspection room, with a set of gauge pins laid out in order of size on a felt strip beside it and a caliper behind, under cool diffuse light. — Those holes are either in position or they are not, and a pair of coordinate dimensions cannot say which. That gap between what the drawing states and what the part has to do is the whole reason geometric tolerancing exists.

The square zone problem

Locate a hole with 50 ± 0.1 across and 30 ± 0.1 up, and you have drawn a square tolerance zone 0.2 mm on a side.

But the hole does not care about x and y. A bolt passes through it or it does not, and that depends on how far the hole is from where it should be in any direction — a radius.

A comparison of two tolerance zones for the same hole. On the left, a square zone 0.2 millimetres on a side produced by plus or minus 0.1 in two directions, with the corner distance from the centre marked as 0.141 millimetres and hatched regions showing where parts are accepted although they are further out than the axes allow. On the right, a round diameter 0.28 zone that circumscribes the square, with the extra accepted area shaded and labelled as 57 per cent more tolerance for the same functional requirement. Below, two rejected and accepted example holes are plotted in both zones to show a part that the square zone rejects and the round zone correctly accepts. — The square zone is wrong in both directions at once — generous in the corners, mean along the axes. The round zone describes what the bolt actually experiences, and happens to be 57 % larger.

The square zone is 1.41× further out at the corners than along the axes. So it accepts parts that are worse than the limit you intended, and rejects parts at 0.12 mm off-axis that would have assembled without complaint.

Describing the requirement correctly — a round zone — gives about 57 % more tolerance for free, and it is the right 57 %.

Reading a feature control frame

An annotated feature control frame reading position, diameter 0.2, maximum material condition, datum A, datum B, datum C. Each compartment is called out below with its meaning: the geometric characteristic symbol, the shape of the tolerance zone, the tolerance value, the material condition modifier, and the primary, secondary and tertiary datum references in order of precedence. A second panel shows the same frame attached to a hole on a plate and the resulting cylindrical tolerance zone about true position. — Read it left to right as a sentence: what is controlled, by how much, under what condition, relative to what — in that order of datum precedence.

| ⌖ | ⌀0.2 Ⓜ | A | B | C |
  │     │      └── relative to what, in precedence order
  │     └───────── by how much, and under what condition
  └─────────────── what is being controlled

A frame with no datum compartment controls the feature against itself only — that is what form controls are.

The fourteen characteristics

Category	Controls	Datum?
Form — straightness, flatness, circularity, cylindricity	The feature against itself	Never
Profile — profile of a line, profile of a surface	Form, orientation and location together	Optional
Orientation — perpendicularity, parallelism, angularity	Attitude relative to a datum	Always
Location — position, concentricity, symmetry	Where the feature is	Always
Runout — circular runout, total runout	Surface behaviour as the part rotates	Always

Maximum material condition — where the free tolerance comes from

This is the idea that converts GD&T from a drafting formality into money.

A hole is at its worst case for assembly when it is at its smallest. That is maximum material condition — the most material, the least clearance. So that is the condition the stated position tolerance is set for.

If the hole comes out bigger, the extra clearance is genuinely there, and it is released back as bonus position tolerance.

Hole:      ⌀10.0 / 10.4
Position:  ⌖ ⌀0.2 Ⓜ  A B C

Hole at 10.0  ->  0.2 + 0.0  =  0.20 position tolerance
Hole at 10.2  ->  0.2 + 0.2  =  0.40
Hole at 10.3  ->  0.2 + 0.3  =  0.50
Hole at 10.4  ->  0.2 + 0.4  =  0.60

Where this goes next

The datum letters in the frame are doing far more work than they appear to — see datums and datum reference frames. What happens when several toleranced features stack up in an assembly is tolerance stacks. And the reason any of it is worth the trouble starts with engineering drawings and tolerances.

What to take away

Plus-minus location gives a square zone; function needs a round one.
The round zone is about 57 % larger, and it is the correct 57 %.
Read a feature control frame as a sentence: what, how much, under what condition, relative to what.
Form controls never take a datum. Everything else does.
Profile of a surface controls form, orientation and location at once — the workhorse for sheet metal and castings.
Circular runout passes a cone; total runout does not.
Ⓜ releases bonus tolerance as a feature departs from maximum material condition, because that clearance is really there.
Do not apply Ⓜ to sealing, bearing or alignment features.