A tolerance on a drawing is a cost decision. Every thousandth tighter than the process naturally holds means slower machines, more inspection or a secondary operation — and a title block copied from a machining drawing can quietly double the price of a sheet-metal part. Here is how to tolerance formed and welded parts so they fit and still cost what they should.
Want a design-for-fabrication review on your drawing? Call 601.892.5017 or email collin.t@fabtekindustries.com — send the model or drawing and our engineers will mark it up.
- Set title-block tolerances to what the process holds: about ±0.010″ on cut features, ±0.015–0.030″ across bends, ±1/16″ on weldments, and ±1° on bend angles. Tighten only the features that need it.
- Tolerance stacks with every bend. Dimension features that must fit each other from the same datum, and on the same flat where possible, rather than chaining dimensions across several bends.
- Use positional tolerance for hole patterns that mate with other parts, and avoid flatness call-outs on large thin panels unless the panel is stiffened or machined.
A title block that fits the process
| Feature | Realistic general tolerance | Governs |
|---|---|---|
| Laser-cut features on one flat | ±0.005–0.010″ | Holes, slots, cutouts, profile |
| Dimensions across one bend | ±0.010–0.015″ | Flange length, hole-to-bend |
| Dimensions across several bends | ±0.020–0.030″ | Box outside dimensions |
| Bend angle | ±1° (±0.5° with measurement) | All formed features |
| Welded assembly | ±1/32–1/16″ | Frames, cabinets, weldments |
| Structural members | Per AISC Code of Standard Practice | Length, holes, camber |
Typical of a well-equipped fabrication shop; see When a Fabricated Part Needs Machining for what milling and turning hold.
The most common mistake is a machining title block — “.XX ±0.010, .XXX ±0.005” — on a formed and welded part. It forces the fabricator to either quote inspection and rework the part doesn’t need, or take exception to the drawing. A separate title block for sheet metal and weldments, or a general note that sets fabrication tolerances, prevents both.
ISO 2768 general tolerances
Metric drawings often reference ISO 2768-1 instead of a title-block table. Class m (medium) is the usual choice for fabricated parts:
| Nominal length | ISO 2768-m linear | ISO 2768-m angular (shorter leg) |
|---|---|---|
| 0.5–6 mm | ±0.1 mm | up to 10 mm: ±1° |
| 6–30 mm | ±0.2 mm | 10–50 mm: ±0°30′ |
| 30–120 mm | ±0.3 mm | 50–120 mm: ±0°20′ |
| 120–400 mm | ±0.5 mm | 120–400 mm: ±0°10′ |
| 400–1000 mm | ±0.8 mm | over 400 mm: ±0°5′ |
| 1000–2000 mm | ±1.2 mm | — |
| 2000–4000 mm | ±2.0 mm | — |
ISO 2768 was written for machined parts, and its tighter angular limits on long legs can be hard to hold on formed sheet. Many fabricators ask that bend angles be tolerated separately (±1°) and that welded assemblies reference ISO 13920, the general-tolerance standard for welded constructions.
Stack-up across bends
Each bend adds its own variation: the flat-pattern calculation, the material’s actual thickness and springback, and back-gauge position. A dimension that crosses one bend carries one bend’s worth of variation; a dimension chained across four bends carries four. That is why the outside width of a formed box is naturally looser than the spacing of two holes on the same flat. Design for it: put mating holes on the same flat where possible, dimension from a single datum instead of chaining, and where a feature on one flange must line up with a feature on another, consider slotting one of them or specifying a hole pattern that is located after forming.
Datums and dimensioning formed parts
Pick datums the fabricator can actually locate: a formed edge, a large flat face, or two holes in the main flat, not the center of a bend radius. Dimension flanges consistently to the inside or outside — say which — because the difference is one material thickness. Dimension formed parts in their formed state, and let the fabricator generate the flat pattern from the model or its own bend tables (Part 3). Avoid dimensioning to tangent points of bend radii, which cannot be measured reliably.
Where tight tolerances earn their cost
Tighten tolerances on the features that mate with something else: hole patterns that bolt to equipment, bus bar or another part (a positional tolerance to a datum is clearer than ± coordinates); door and panel openings that must seal against gaskets; mounting interfaces for breakers, relays and transformers; and machined faces. Leave everything else at the general tolerance. Be cautious with flatness on large, thin panels: sheet has residual stress, welding and powder cure add more, and a flatness call-out tighter than the panel’s stiffness can hold forces added stiffeners or machining.
How to write it
“Unless otherwise specified: sheet metal features on a common flat ±0.010″; dimensions across bends ±0.020″; bend angles ±1°; welded assemblies ±1/16″; inside bend radius per fabricator’s standard tooling, approximately equal to material thickness. Flange dimensions are to the outside. Hole patterns marked ‘A’ shall be located within 0.015″ true position relative to datums B and C. Break sharp edges.”
How FabTek handles it
FabTek’s engineering group reviews tolerances on every new drawing during DFM review and flags call-outs that will add cost without adding function, before the part is quoted and built. Parts are cut from nested flat patterns on the fiber lasers, formed on CNC brakes with angle correction, and inspected to the drawing under ISO 9001:2015; features that need machining tolerance go to the CNC mills.
Frequently asked questions
What tolerance should I put on a sheet metal drawing?
Match the tolerance to the process: about plus or minus 0.005 to 0.010 inch for cut features on one flat, plus or minus 0.010 to 0.030 inch for dimensions across bends, plus or minus 1 degree on bend angles and about plus or minus 1/16 inch on welded assemblies. Tighten only the features that mate with other parts.
What is ISO 2768-m?
ISO 2768-1 class m is the medium general-tolerance class for linear and angular dimensions without individual tolerances, for example plus or minus 0.3 mm from 30 to 120 mm and plus or minus 0.5 mm from 120 to 400 mm. It was written for machined parts, so fabricated parts often add separate bend-angle and weldment tolerances.
Why do sheet metal tolerances stack up?
Each bend adds variation from the flat-pattern calculation, material thickness and springback, and back-gauge position. A dimension chained across several bends accumulates each bend's variation, so it is looser than a dimension between features on the same flat.
Should flanges be dimensioned to the inside or outside?
Either works if the drawing says which and is consistent; the difference is one material thickness. Outside dimensions are common for enclosures and boxes, inside dimensions where a component must fit inside the formed part.
