A cabinet door crossed my desk last quarter with every hole dimensioned from the left cut edge. The model was clean, the title block tolerance was in place, the finish note read "BLACK POWDER COAT." We built it and the door sat proud of the frame on the hinge side. The bend was fine; the sheet metal drawing dimensioning was not. Tying the hole pattern to a cut edge rather than the bend line let accumulated bend allowance push the whole pattern off. The fix was one datum change — after a re-cut and two lost weeks. Most RFQ rework starts there: in what the drawing says, and what it omits.
Key takeaways
- Dimension and datum the formed state, not the flat blank.
- Call out bend direction on the print; one arrow plus a section ends the most common clarification email.
- Tighten only what makes parts fit, seal or ground; let a general tolerance standard carry the rest.
- Name the cosmetic faces. "To supplier standard" is not a requirement.
- Give coating by colour system and code, plus gloss target and measurement geometry.
- Say whether a substitute material or thickness is acceptable. Silence reads as approval.
- What the print does not say, you did not ask for. We can flag the gap; we do not certify the design.
Why sheet metal drawings come back with questions
Rejected prints are rarely drawn wrong. They are lopsided, in one of two directions.
Over-specified. Every cut edge length, bend radius and non-functional slot carries a two-decimal tolerance. The supplier prices in dedicated setups, 100% inspection and a scrap allowance.
Under-specified. Geometry complete, intent silent: nothing says which face is cosmetic, which side the clinch nuts sit on, or whether the hole pattern is measured from the bend or the edge. The estimator guesses.
The two directions cost you in different places, and neither of them shows up as a line item:
| What the print does | What the estimator reads | What it costs you |
|---|---|---|
| Tightens every cut edge and non-functional slot to two decimals | Dedicated setups, 100% inspection, a scrap allowance | A unit price that loses bids the geometry could have won |
| Leaves hole-to-hole on a mating pattern to the general block | Standard process, no special control | A first article that assembles with a tapered punch and then a re-cut |
| Names no cosmetic face | Every face gets graded alike | A rejection you cannot defend, or a panel you have to accept |
| Names no coating exclusion | Coat everything | Threads and grounding pads reworked on the bench, on every unit |
| Silent on material or thickness substitute | An equivalent substitute is fine | A part that meets the print and fails in the product |
That is the whole job of sheet metal drawing dimensioning: not precision, but removing the freedom to build two different parts from one file.
The test we run before quoting: could two competent shops build different parts that both pass this print? If yes, it is a callout problem. File formats are a separate matter — sheet metal RFQ checklist.
If you want that test run before the print goes out, send the model and the drawing for a free CAD and DFM review — we mark up the callouts we would question and quote within 24 hours. The whole workflow is in the sheet metal process and DFM hub.
Start with the state: formed part or flat pattern
Sheet metal is the rare process where one part has two legitimate geometries. Pick one as the definition and mark the other reference. It is the one decision in sheet metal drawing dimensioning that everything else depends on.
Dimension the formed state. Datums belong on surfaces that mate, seal or get inspected: the outside of a bend, a mounting face, the door opening. A flat-pattern dimension transfers every bend allowance in the chain onto your hole pattern.
Why it bites. A hinge pattern dimensioned from the flat blank edge is right on the flat and wrong once formed, by the accumulated allowance of each bend in between. Dimension it from the bend line or the outside of the bend and the stack-up collapses to a single tolerance.
The failure is rarely dramatic when it happens. A 19-inch shelf that crossed my desk last year had its rail holes dimensioned from the rear cut edge, with two bends in between. On the flat the pattern was exact. Once formed, the rail holes sat short across the whole run, and every unit had to be re-cut on the laser from a corrected DXF. Nothing about the part was hard to make. The origin was in the wrong state, and nobody found it until the shelf met the rack.
Call out bend direction. Do not rely on the reader opening the model: a bend direction arrow on the view, backed by a section or a note. On symmetric parts name the cosmetic side; a part bent the wrong way is scrap rather than rework.
A bend callout that survives an RFQ usually fits in three lines:
BEND UP — SEE SECTION A-A
ALL HOLES DIMENSIONED FROM OUTSIDE OF BEND
THIS SIDE COSMETICThe arrow says which way, the origin note says where measurements start, and the cosmetic note tells the handler which face does not go down on a bench. Three lines, and the most common clarification email in the program stops arriving.
Mark any flat-pattern DXF FLAT PATTERN — REFERENCE ONLY; FORMED DIMENSIONS GOVERN. Bend behaviour — springback, flange limits — sits in the bending guide.
What to tighten, and what to leave to the general tolerance standard
Name a general tolerance standard in the title block — ISO 2768-1 or an ASME Y14.5 general profile note, current edition, no clause numbers — and deviate only where a function demands it. Every individually tightened dimension is another setup, another check, another reason to scrap a good part.
Two things about that title block line are worth knowing before you write it.
ISO 2768 Part 2 is withdrawn. It was cancelled and replaced by ISO 22081, and the replacement also changed the method: where the old Part 2 offered fixed tolerance classes you could inherit by letter, ISO 22081 expects you to write the general geometrical value yourself. There is no default class to inherit, so a bare "ISO 2768" reference on a new drawing leaves the geometrical half undefined.
Undated references drift. An undated citation means the current edition applies. A drawing that says "ISO 2768-mK" therefore points its geometrical half at a document ISO no longer maintains. If you need a meaning that does not move, date the reference, or move the geometrical half onto ISO 22081 and write the value in.
There is also a rule here that cuts in the buyer's favour and is easy to forget: under ISO 2768-1, exceeding a general tolerance is not by itself grounds for rejection unless the function of the part is impaired. If you intend any overshoot to be rejected on principle, say so on the purchase order. Silence defaults to the function test, and that is the harder argument to win.
| Dimension or callout | Tighten it when | Leave it to the general tolerance standard when |
|---|---|---|
| Hole-to-hole on a mating pattern | It bolts to a second part and misalignment blocks assembly | The holes are non-functional venting or weight relief |
| Feature to bend line | A hole, latch or gasket lands on or near the bend | The feature sits in the middle of a flat field |
| Flatness of a gasket or sealing face | An EMI gasket, IP seal or door stop needs continuous contact | The face carries nothing but air |
| Position of self-clinching hardware | A stud or nut must line up with a mating clearance hole | Hardware is placed by hand at assembly |
| Grounding stud location | Bonding depends on position and bare metal contact | The stud only routes cables |
| Bend angles | Two panels close on a shared seam, or a door must sit flush | The angle only clears an internal component |
| Overall envelope | The assembly slides into a rack or fixed aperture | The part is free-standing |
| Non-mating cut edge lengths | Almost never | Almost always — the classic over-tolerance |
| Inside bend radii | Almost never, unless a tool is already committed | Standard tooling radii are cheaper and more repeatable |
| Welded assembly dimensions | Only for machined mating faces after weld | Use a current welding tolerance standard (ISO 13920) or general geometrical tolerance standard (ISO 22081) |
Two counterexamples, and they are the two halves of the table above.
Tightening everything on a bracket turns a laser-and-brake job into one that carries a CMM report, and the price loses the bid. It happens in a recognisable way: an industrial control bracket arrives with every feature held to two decimals, including four slots that exist only to take weight out of the part. Nothing on it is difficult, but the print now implies a second setup to hold those slot widths and a full dimensional report to prove it. The quote comes back in a different bracket of money, the buyer asks why, and the answer is a tolerance nobody needed. Two days later the same part returns with four decimal places removed and the price falls. The part never changed. What the print asked us to guarantee did.
Leaving hole-to-hole on a rack-mount pattern to the general block means the first article assembles with a tapered punch.
Numeric bands live in the sheet metal tolerance guide; the cost mechanics in the DFM cost reduction guide.
Hole and feature callouts that decide whether the part builds
Hole to bend. Dimension from the bend line or the outside of the bend, and state which — never from a cut edge when the function is relative to the bend. What the minimum distance should be is answered in the DFM design guide; what matters here is that the origin is stated.
Hole to hole. Dimension patterns from one datum, not chained. Chaining accumulates every tolerance across the pattern, and a ten-hole rail is where it shows: ten chained steps each carry their own tolerance, and it is the tenth hole that misses its mating part.
Self-clinching hardware. Three items: fastener by performance spec or part number, direction (which face ends flush), and whether it installs before coating. Coated hardware without a masking note has coated threads, which change assembly torque — see the self-clinching fastener design guide.
4x S-M4-1ZI, INSTALL BEFORE COATING
FLUSH SIDE: INSIDE FACE
MASK THREADS DURING COATINGThreads. State thread, class, and whether a tapped through-hole is acceptable or you want a clinch nut, plus whether holes are gauged after coating — see the assembly fastener selection guide.
Edges. Deburr is a callout, not a default: BREAK ALL EDGES; NO BURR ON SEALING FACE, per the edge break and deburring guide.
Enclosure-specific callouts most shops never get
Generic prints fail here. An enclosure carries requirements a bracket does not, and this is where sheet metal drawing dimensioning earns its keep.
Define the A-surface. Name the faces in a view and say how they are judged: inspection distance, lighting, whether minor handling marks are acceptable. With no named faces, every mark becomes a dispute. Classes in the cosmetic surface class guide.
Write it as a named list, not as an adjective:
FACE A (COSMETIC): FRONT, TOP, DOOR OUTER
FACE B (NON-COSMETIC): REAR, BOTTOM, INTERIOR
FACE A INSPECTED AT 1 m, DAYLIGHT, 5 s PER FACE
MINOR HANDLING MARKS ACCEPTABLE ON FACE B ONLYThat block settles four arguments before they start: which faces matter, how close the inspector stands, what light they stand in, and whether a scuff is a defect. "Appearance to supplier standard" settles none of them — and it is the sentence that produces the worst email thread in a program, the one where a panel is rejected against a rule nobody wrote down.
Door gap and flushness. Call out the nominal gap and which face is the flushness reference; a door flush at the hinge and proud at the latch is a print problem, not a fitting one. Large-door flatness needs its own callout and its own method: flatness and oil canning guide.
Weld and grind grade. Name the weld class and reference your acceptance criteria, then the finish: GRIND FLUSH, 120 GRIT, DIRECTIONAL, MATCH ADJACENT. For post-weld dimensions use a current welding tolerance standard such as ISO 13920, or ISO 22081 — not ISO 2768 Part 2, which is withdrawn. ISO 13920 was itself reissued as a second edition in 2023, so a drawing citing the 1996 edition is pointing at another withdrawn document. Visual levels in the weld appearance acceptance criteria guide.
Grounding. Call out stud location, the coating exclusion around it, and the bonding requirement; a stud buried under powder does not ground. Say whether door-to-frame continuity is verified on every door or by sampling. Detail in the enclosure grounding and bonding design guide.
Have a door or a full enclosure to release? Send the model and print for a free CAD and DFM review — we will tell you which of these callouts are missing before you commit to tooling. See how we work as a custom sheet metal enclosure manufacturer.
Finish callouts: colour, masking and coating exclusions
RAL is a commercial colour fan published by RAL gGmbH, not an ISO, EN or national standard — write it as a colour reference, never as a "reference standard." That distinction is one of the few places where sheet metal drawing dimensioning touches a document that was never a standard to begin with. Give the system and code: RAL CLASSIC 7035. Add the gloss target and the measurement geometry: gloss per ISO 2813 or ASTM D523 at 60°, 20° for high-gloss and 85° for low-gloss. Batch expectations in the powder coating colour match guide.
The geometry on that note is not a formality. Those two standards use three angles because one of them stops resolving at the extremes: 60° is the general geometry, 20° separates high-gloss films that all read alike at 60°, and 85° separates near-matt films. A note that names a gloss value with no angle can be met three different ways. One more caution worth carrying into the RFQ: the ISO 2813 and ASTM D523 method is not suitable for metallic coatings, so a metallic or sparkle powder has to have its appearance defined some other way — a retained panel, submitted in advance and agreed in writing.
Masking. Hatch the zone, label it, and say whether it is masked during coating or coated and machined afterwards; the two leave different edges. See the hang points, vent holes and masking guide.
Exclusions. List them: grounding pads, threads, gasket seating faces, hinge bearing surfaces, label areas. NO COATING ON GROUNDING PADS AND THREADS removes a bench rework step from every unit.
Notes that save a round trip
Short, numbered, and answering questions you know are coming. Every note below exists because sheet metal drawing dimensioning is read by a shop, not by a CAD system.
- Revision and authority. Revision in the title block plus
3D MODEL REFERENCE ONLY — DRAWING GOVERNS, or the reverse if you mean it. See the revision control and ECN guide. - Material and thickness. Call out material by specification, give thickness as a value, then say whether a substitute is acceptable:
SUBSTITUTE: NOT PERMITTED WITHOUT WRITTEN APPROVAL. Grades in the material selection guide. - First article. If you want a report before the batch, say so and name what gets measured — FAI and PPAP guide.
- Packing and inspection. Specify face protection for cosmetic panels and list the characteristics you want reported; the rest follows our standard plan in the quality control and inspection guide.
Where the drawing responsibility sits
A drawing review has a boundary, and it is worth stating plainly, because it decides who owns a bad part.
What we do. We read the print, build to it, and give you DFM opinions: where a callout will cost money, where a dimension will not hold, where a missing note will turn into a dispute. Free CAD and DFM review, and a quote within 24 hours.
What we do not do. We do not certify a design, sign a drawing off as conforming to a standard, or take responsibility for the load, thermal, EMI or safety performance the print implies. We have not seen the product it goes into. A stamped drawing from your engineer of record, and any product-level compliance work, sits with you and your notified body.
What follows from that. A print we quote without comment is not a print we have approved. If a callout is missing, the absence is a commercial gap, not a warranty. That is the reason this article keeps asking you to write things down: in a dispute, the print is the only record both sides can read.
Frequently asked questions
Should I dimension sheet metal parts in the flat or the formed state?
Dimension and datum the formed state and mark the flat pattern reference only. Features dimensioned from a flat blank edge pick up the accumulated bend allowance of every bend in between, so a pattern that is perfect on the flat ends up off in the assembly.
Do I need to call out bend direction on every bend?
Yes, whenever it is not obvious from one view. Put a bend direction arrow on the drawing and back it with a section or a note. A part bent the wrong way is scrap rather than rework, and it is a leading cause of first-article rejection.
How do I define a cosmetic A-surface face on a drawing?
Name the faces in a view and label them, then state how they are judged: inspection distance, lighting, and whether minor handling marks are acceptable. A note saying appearance is to supplier standard sets no requirement.
Can I use ISO 2768 for welded assembly dimensions?
Use ISO 2768-1 for general tolerances on non-welded features, but not ISO 2768 Part 2 for welded dimensions, because it is withdrawn. Point welded envelope dimensions to a current welding tolerance standard such as ISO 13920, or to ISO 22081.
How should I call out masking areas for powder coating?
Hatch the area on the relevant view, label it, and state whether the zone is masked during coating or coated and machined afterwards. Also list coating exclusions explicitly, such as grounding pads, threads and gasket seating faces.
Conclusion
Sheet metal drawing dimensioning is a communication problem before it is a tolerancing one. Three things remove most round trips: datum the formed state, call out bend direction and hardware orientation, and tighten only what makes the product fit, seal or ground.
Releasing an enclosure or cabinet? Send the model and print for a free CAD and DFM review — we mark up the callouts we would question and quote within 24 hours. Start at the sheet metal process and DFM hub or see how we work as a custom sheet metal enclosure manufacturer.