Engineering Drawing Checklist: 8 Checks Before You Release

A drawing is a contract. The supplier makes what it says, the inspector checks what it says, and anything it doesn't say gets decided by someone else, usually at the worst moment. "Material: aluminium", "no burrs", a title block with ISO 2768-fH and a 0.3 mm chamfer nobody toleranced: each one turns into a phone call, a deviation or a scrapped batch.

This is the release checklist we used in R&D, updated to current ISO standards. Eight checks, in the order you meet them on the sheet.

The checklist at a glance

Dimension function first, then machine it in your head

When I start dimensioning a part, I always go function first:

1. Datums, on the surfaces that locate the part in its assembly.
2. Geometric tolerances the function needs, related to those datums.
3. Dimensional tolerances on the functional sizes and fits.
4. Specific surface textures, beyond the general one in the title block.
5. Everything else, covered by the general tolerances.

In that order, function is on the sheet before it gets crowded, and the general tolerance only covers what doesn't matter.

Then, as a check, I put myself in the machinist's place and machine the part in my head, operation by operation. Every time I need a value that isn't on the sheet, a dimension is missing. Overall dimensions are the classic gap: rarely functional, but the shop needs them to choose the raw stock. I add them in parentheses as auxiliary dimensions (ISO 129-1), for information, without tolerance.

Title block: general tolerances and tolerancing principle

The general tolerance in the title block covers every dimension without its own tolerance, so it must match how the part is made. A machining standard on a molded part is either impossible or meaningless.

Small dimensions fall outside the tables. ISO 2768-1 starts at 0.5 mm, so a 0.3 mm chamfer has no general tolerance. Tolerance it, or add a title block line such as "<0.5 mm: ±0.05".

ISO 8015 and functional dimensioning

Our rule: every new design is dimensioned functionally per ISO 8015 from the first prototype drawing. Datums on the surfaces that locate the part in its assembly, positions and orientations related to them. Old drawings under revision don't have to be converted.

ISO 8015 sets the independence principle: a ⌀7 ±0.02 controls local size, not form. If that diameter must fit in a bore, add the envelope requirement Ⓔ (ISO 14405-1) or a form tolerance. Since 2011, ISO 8015 applies by default on any ISO GPS drawing, but writing it in the title block removes all doubt. Symbols are covered in GD&T explained.

The myth of the nominal value

On a ±0.05, the old belief goes, the machinist aims for the middle, so the design can count on the nominal. Sometimes. Never guaranteed. The contract is the whole zone. Setup slightly off and every part at the lower limit: good parts. Tool wear drifting them to the upper limit: still good parts. The drawing says so.

The design has to work anywhere in the tolerance, including mating parts at opposite extremes. If it only works near nominal, the tolerance is wrong, not the machinist.

Material and surface texture

Material: one per drawing, fully designated, no brand names (write PMMA, not Plexiglas). "Aluminium" leaves the choice to the supplier.

Surface texture: a general symbol is always on the drawing, in Ra, with specific symbols where the function needs better (Ra 0.8 on a seal). The rules now sit in ISO 21920-1, which replaced ISO 1302; the symbol is unchanged. Put the treatment on that symbol, not in a "Surface finishing" box: "Colorless anodized 15–20 µm" over Ra 1.6. More in Ra vs Rz.

Edges and burrs: replace "no burrs" with ISO 13715

"No burrs" is the most common note on a drawing and one of the least useful. Under what magnification? Nobody can measure it, so nobody can accept or reject against it. ISO 13715 gives edges a symbol with values. External edge: − is material removed (edge break), + a burr allowed. Internal edge: + is material allowed in the corner (tool radius), − an undercut.

One general symbol near the title block for all edges, individual ones where needed. If a burr can't be avoided, at a parting line for example, state how much is acceptable with the same symbol. Now it's measurable.

Special characteristics: make the DFMEA visible on the drawing

A critical characteristic in the DFMEA is useless if the drawing doesn't show it. In the template behind this checklist, a high-severity characteristic that couldn't be tested 100% in production was marked CC, and the title block stated the capability: Cpk ≥ 1.67 for CC, Cpk ≥ 1.33 for SC. In pure design work I rarely see these thresholds. They show up in industrialization, when optimizing existing machines, or in the specifications of large industrial customers, so take the values from your customer's requirements.

Typical case: a sealing surface where a scratch means an external gas leak, severity 9. The diameter, the Ra 0.8 and the "no marks" zone all get the CC mark, so the supplier knows before quoting that a capability study is part of the job. Left off the drawing, that dimension is sampled like any other ±0.05, and the first sign of a problem is a leak in the field.

From the shop floor: one drawing, before and after review

A small turned support ring in anodized aluminium. On paper it looked finished. The review found seven corrections:

1. Inspection balloons removed from the design release.
2. "ALU" replaced by the alloy, 6060 (EN AW-6060 in full).
3. Anodizing moved to the surface symbol, with its thickness: colorless, 15–20 µm.
4. "<0.5 mm: ±0.05" added for dimensions below the general tolerance table.
5. General edge symbols added: −0.02/−0.07 edge break outside, +0.05 inside.
6. Functional dimensioning: datums, position and coaxiality, theoretically exact dimensions, envelope Ⓔ on the two fitting diameters, ISO 8015 in the title block.
7. Specific surface requirements written in Ra.

None of these changed the part's geometry. All of them changed what the supplier would quote, make and check.

The takeaway for the shop floor

Before you release, read the drawing as the supplier will: only what is written counts. Every value in the tolerance zone is a good part, so design for the extremes. And if a part refuses to be toleranced functionally, go back to the design, not the drawing. More designs for people who live in drawing reviews in the quality engineer collection.

FAQ

About the author

Gabriel Weider is a mechanical engineer with 15 years in special machines, CAD, medtech and regulated environments. He still works full-time as an engineer and designs every grabNade shirt. Read his story.