Opening question
"Left is Correct, Right is Wrong" — Do You See Why?
Chapter 2 of geometric tolerancing opens with a question about a drawing. Two versions of the same part show ± specifications — one correct, one wrong. The difference is not obvious at a glance, but it reveals one of the most important principles in dimensional control.
Fig.01 — Correct specification (left) vs. incorrect specification (right)
Left: hole diameter and slot width are sizes — "large" or "small" can be said — ± is valid.
Right: hole center position and step height are not sizes — "large" or "small" cannot be said — ± is not valid.
The correct left-side specification controls the hole diameter, slot width, and plate width — all of which can be described as larger or smaller. The incorrect right-side specification attempts to control the hole center-line position, the slot center plane, and a step height — none of which can meaningfully be called large or small.
Positions, center planes, and step heights cannot be toleranced with ± —
they require geometric tolerancing (GD&T).
This distinction — what can and cannot receive a ± specification — is the core of Chapter 2.
Definition
What Is a Size Feature?
The word "feature" is the English translation of the Japanese term 形態 (keitai). In 3D CAD, you extrude a boss, drill a hole, cut a slot — each of those operations is a feature. A feature is simply a distinctive portion of a part.
Among all features, those defined by a size are called size features. Only size features may receive a ± size tolerance. Everything else must be controlled with geometric tolerancing.
Important caveat
Even if a feature is cylindrical or consists of two parallel planes, if it is defined by a geometric tolerance rather than a size, it is no longer a size feature. The shape alone does not determine size-feature status — what matters is whether it is defined by a size specification.
The five eligible forms
There Are Exactly Five Size Features
In principle, ± tolerancing can be applied to only the following five feature types.
In daily shop floor work, the cylinder (bores and shafts) and opposed parallel planes (slot widths, plate thicknesses) account for virtually all practical size features. Cone and wedge are angular size features — measurable with a universal bevel protractor.
Fig.02 — The common structure shared by all five size features
All five size features share the same geometric property: a center (point, line, or plane) from which opposing arrows can be drawn outward. This is what makes them measurable as a "size."
Effect on molded and cast parts
Parts made by injection molding or casting typically have draft angles on most surfaces. This means the number of genuine size features is greatly reduced — only holes and slots machined after molding qualify. Most surfaces on such parts must be controlled with geometric tolerancing.
The condition for "opposed parallel planes"
"Opposed" (相対する) means the two planes face each other: parallel, same shape, same position. It is not enough to simply be flat and parallel — they must be directly opposite one another so that a gauge can be inserted between them.
| Configuration | Verdict | Reason |
|---|---|---|
| Facing each other — same shape, same position | ✔ Size feature | Typical slot/plate thickness. A block gauge fits between them. |
| Same direction (not facing) | ✘ Not a size feature | A gauge cannot be inserted; no opposition exists. |
| Facing — same shape, but offset in position | ✘ Not a size feature | No corresponding area to measure across. |
| Partially opposed (e.g., stepped surfaces) | △ Use caution | Not a clear error, but ambiguous. Consider using a continuous size feature (CT) or geometric tolerance. |
Scope of tolerancing
The Tolerance Framework
"Everything that is not one of the five size features must use geometric tolerancing" — that statement is half correct and half misleading. The full picture is this:
All features (geometric tolerancing applicable)
5 size features — ± size tolerance OR geometric tolerance (either is valid)
Features requiring geometric tolerancing only
* Surface texture (Ra, Rz) and edges are controlled by separate standards — not by size tolerances or geometric tolerances.
The five size features can validly use either a ± size tolerance or a geometric tolerance. The choice depends on function, cost, and the measurement method available.
Cost perspective
Measuring a bore diameter with a cylinder gauge (a size measurement) costs far less than measuring it with a CMM under a roundness or cylindricity tolerance. However, switching from ± to a geometric tolerance does not automatically raise cost — a step height controlled with a height gauge is perfectly affordable. Match the tolerance type to the actual measurement method, not to a blanket rule.
Features that cannot be controlled by either type of tolerance
Edges (sharp corners) are a special case: they are excluded from both size tolerancing and geometric tolerancing. Two reasons explain why:
| Reason | Explanation |
|---|---|
| Measurement problem | A CMM stylus cannot reliably contact a sharp edge. Even under a microscope, finding the "intersection" still requires measuring the two surfaces separately — the edge itself is never directly measured. |
| Definition problem | At an edge, the surface normal is undefined. The ISO 2692 vector-based definition of size therefore cannot be applied. |
Practical workaround
Leaving even a tiny straight (cylindrical) land eliminates the edge problem entirely. Examine commercial screw heads: even countersunk (flat-head) screws have a small straight section below the head face. When edge control is needed, specify the two adjacent surfaces and derive the edge position from them.
Practical judgment method
The Gauge Principle — Field Judgment in Practice
When you are unsure whether a feature qualifies as a size feature, there is a reliable practical test used on the shop floor:
If a plug gauge, ring gauge, block gauge, snap gauge, or pin-type micrometer can grip or straddle the feature, it is a size feature. If not, it is not.
Using the gauge principle, you can make an instant judgment from physical intuition — without consulting standard clauses one by one.
Reference table
Judgment Examples by Feature Type
The table below summarizes common feature configurations and their size-feature status. ✔ = size feature, △ = use caution, ✘ = not a size feature.
| Feature | Verdict | Reason / Recommended approach |
|---|---|---|
| Round hole (cylinder, internal) | ✔ | Plug gauge inserts and straddling is possible. Classic size feature. |
| Round shaft (cylinder, external) | ✔ | Ring gauge straddles it. Classic size feature. |
| D-cut shaft or hole (more than half remaining) | ✔ | Gauge can still be applied. Size feature remains valid. |
| Less than half a circle (arc only) | ✘ | Gauge cannot seat stably. Use a profile tolerance (surface profile). |
| Slot width / plate thickness (opposed parallel planes) | ✔ | Snap or block gauge applies. Classic size feature. |
| Two surfaces facing the same direction | ✘ | No opposition; gauge cannot be inserted. Use profile tolerance (linear distance). |
| Step height | ✘ | No opposing surface. Use profile tolerance. |
| Hole center position | ✘ | Cannot be described as large or small. Use position, perpendicularity, etc. |
| Radius (R) | ✘ | No opposing surface for the gauge; measurement error accumulates. Use profile tolerance. |
| Corner edge / chamfer | ✘ | Cannot be toleranced by size or geometric tolerancing. Specify adjacent surfaces. |
| Countersink (tapered hole without straight land) | ✘ | Gauge cannot seat. Specify diameter at a reference depth + angle. |
| Elongated hole (oblong slot) | △ | If both end radii are identical, close to a size feature. If different, JIS B 0420 notes "ambiguity exists." Verify carefully. |
| Toroidal inner diameter (donut bore) | ✔ | Two-pin contact measurement is possible. Size feature. |
| Grooved cylinder (continuous size feature) | △ | Can be designated as a Continuous (Collection) Size Feature (CT) per JIS B 0420-1:2016. |
| Axial length between shoulders on a shaft | ✘ (mostly) | Axial step = no opposing parallel planes in that direction. Use profile tolerance. |
| Bent / formed sheet metal profile | ✘ (mostly) | Opposed parallel planes rarely exist in bent forms. Use geometric tolerancing. |
Common shop floor discrepancy
It is not unusual to encounter drawings where a ± size tolerance is specified for a feature that is not actually a size feature — and where the measurement has been carried out with a geometric interpretation all along. Reviewing such drawings often reveals that a simple tolerance re-statement (not a tighter or looser value — just the correct tolerance type) is all that is needed.
Key takeaways
Summary
Point 01
Only 5 features accept ±
Cylinder, opposed parallel planes, sphere, cone, and wedge. In practice, the first two cover almost everything.
Point 02
Use the gauge test
"Can a plug, ring, snap, or block gauge grip or straddle it?" — this single question resolves most real-world cases without consulting standards text.
Point 03
Edges are exempt from both
Edges cannot be controlled by size tolerances or geometric tolerances. Specify the adjacent surfaces; the edge follows.
Point 04
The 5 features accept either type
For the five size features, ± and geometric tolerancing are both valid. Choose based on function, cost, and measurement method — not habit.
The goal of this chapter is to correct the assumption that "any dimension can have a ±." Once you build the mental image of a gauge gripping or straddling a feature, you can judge in an instant — just by looking at the drawing — whether a feature is a size feature or not. The next article will go deeper into the precise definitions of each of the five size features.