Engineering Drawings
You send the same drawing to three shops. Three different parts come back. All three say they built it to print.
A drawing can be dimensionally perfect and still not be a specification. If it doesn’t say what standard the tolerances follow, which projection it’s drawn in, or what “finished” means for that surface, the shop decides for you — and three shops decide three different ways.
What’s actually happening
A dimension without a tolerance isn’t a dimension a machinist can work to — it’s a suggestion with a decimal point. Most drawings don’t tolerance every dimension individually; they lean on a general tolerance note to cover everything else. If that note is missing, there is no tolerance on most of the drawing, whatever the title block looks like — the shop will assume something, and what they assume is not guaranteed to be what you needed.
The same is true of projection angle, units, material specification and finish. None of these are implied by geometry. They have to be stated.
The title block — what has to be there
| Item | Why it can’t be assumed |
|---|---|
| Material + spec (e.g. S235JR, not just “steel”) | Different specs of the same nominal material have different mechanical properties |
| General tolerance note (e.g. ISO 2768-mK) | Governs every dimension you didn’t tolerance individually |
| Projection angle symbol | First-angle and third-angle place views on opposite sides |
| Units | Especially where a client works in inches and the drawing is metric, or vice versa |
| Surface finish default | What “as machined” means if no callout says otherwise |
| Scale, with a clear “not to scale” flag on any view that isn’t | Printed and PDF drawings both get resized in ways that fool a ruler held to the screen |
| Revision letter + date | See revision control, below |
| “Unless otherwise specified” scope line | Ties every default note to the specific callouts that override it |
General tolerances — the note that governs everything else
ISO 2768-1 defines four classes for linear dimensions: fine (f), medium (m), coarse (c), very coarse (v). I checked this table against three independent published sources before using it — the values below match all three.
| Size range (mm) | f — fine | m — medium | c — coarse | v — very coarse |
|---|---|---|---|---|
| 0.5 – 3 | ±0.05 | ±0.1 | ±0.2 | — |
| >3 – 6 | ±0.05 | ±0.1 | ±0.3 | ±0.5 |
| >6 – 30 | ±0.1 | ±0.2 | ±0.5 | ±1.0 |
| >30 – 120 | ±0.15 | ±0.3 | ±0.8 | ±1.5 |
| >120 – 400 | ±0.2 | ±0.5 | ±1.2 | ±2.5 |
| >400 – 1000 | ±0.3 | ±0.8 | ±2.0 | ±4.0 |
| >1000 – 2000 | ±0.5 | ±1.2 | ±3.0 | ±6.0 |
| >2000 – 4000 | — | ±2.0 | ±4.0 | ±8.0 |
This class has no defined tolerance for this size range — ISO 2768 leaves it to be individually toleranced.
A general tolerance class is a default, not a suggestion, and it applies to every dimension on the sheet you didn’t individually tolerance — including ones you forgot were there. A 4000 mm dimension sitting on an “ISO 2768-c” note with no individual tolerance is ±4 mm, whether or not that’s what anyone intended.
Dimensioning logic — chain vs baseline
Chain dimensioning strings each feature off the last one. Baseline dimensioning references every feature back to a single datum edge. They produce the same nominal part and completely different tolerance stack-up.
Four features, each individually toleranced ±0.1 mm. Chain-dimensioned, the worst-case error on the last feature is the sum of every tolerance before it — ±0.4 mm, even though no single dimension was that loose. Baseline-dimensioned, every feature’s worst case is still ±0.1 mm from the datum, because none of them depend on where the previous one landed.
Chain dimensioning isn’t wrong — sometimes the relationship between adjacent features matters more than the relationship to a far edge, and that’s a legitimate reason to chain them. It’s wrong when it’s the default because nobody thought about which relationship actually mattered.
First-angle vs third-angle projection
Germany draws first-angle. The US draws third-angle. The same drawing, read under the wrong convention, puts the top view on the wrong side of the front view — and nothing about the geometry tells you which one you’re looking at except the projection symbol in the title block.
The notes that aren’t optional
- Deburr / break sharp edges — without it, “sharp” is whatever the operator judged safe to handle, part to part.
- Surface finish (Ra) — a number, not “smooth.” If it’s not called out, the shop’s default finish for that process is what you get, and that varies machine to machine.
- Thread callouts, full form — M6×1.0–6H is a specification; “M6 tap” is a guess at class and pitch.
- Weld symbols with a standard reference (e.g. to ISO 2553 or AWS A2.4) — a fillet symbol without a governing standard leaves size and profile to interpretation.
- “Unless otherwise specified” scope statement — ties every default note on the sheet to the specific callouts that override them, and says so explicitly.
Revision control
A drawing changes. The part it describes should change with it — visibly. An unmarked revision is worse than no revision, because it looks authoritative and isn’t. A rev letter, a date, a description of what changed, and ideally a delta cloud on the sheet around the changed area, are what stop a shop building against a cached PDF from three revisions ago.
Why we care
Most of what goes wrong between a drawing leaving my hands and a part coming back wrong isn’t bad geometry. It’s a decision that was never written down, made twice, differently, by two people who both thought they were being reasonable.
I write the projection angle on every drawing that leaves this business, even though it feels obvious to me — because a shop in Ohio and a shop in Stuttgart don’t share the same “obvious,” and I’d rather spend one symbol confirming it than one shipment finding out.