Tight tolerances are the most expensive thing you can ask for on a custom sheet metal part, and they are also the most over-specified. A drawing that calls for ±0.05 mm on every dimension can push the same part's price up 30–50% with no functional benefit — and it will not even guarantee the part holds those tolerances in production. Sheet metal tolerance is the discipline of asking for precision only where the assembly actually needs it.
What Tolerance Can Sheet Metal Actually Hold?
Standard sheet metal fabrication — laser or turret-punch cutting, press-brake bending, MIG or TIG welding, powder coating — can hold surprisingly tight tolerances out of the box, but only on the right features. As a rule of thumb:
- Laser-cut linear dimensions: ±0.1 mm on features held in a single setup; ±0.2 mm across the part. State-of-the-art fibre lasers with modern controllers are tighter still.
- Bend angles: ±0.5° with standard press-brake tooling on simple bends; ±1° on hard-to-access or tight-radius bends.
- Hole diameters: ±0.05 mm typical for laser; ±0.1 mm for punched holes.
- Hole-to-hole positional: ±0.1 mm typical on a single setup; ±0.2 mm is more realistic across multiple setups.
- Flatness: ±0.3 mm per 300 mm is typical on a thin panel; thicker stock holds flatness better.
- Weld assembly tolerances: ±0.5–1.0 mm typical on a small welded assembly; ±1.0–2.0 mm on a large cabinet.
Pushing beyond those windows — say ±0.05 mm on a bend angle, or ±0.02 mm on a hole position — forces the fabricator into secondary machining, extra inspection, hand fitting or part-by-part sorting. Each step adds cost without necessarily adding quality.
ISO 2768: The Default Tolerance Standard
ISO 2768 is the most widely accepted general tolerance standard for sheet metal and machined parts that are not otherwise individually toleranced. It defines four tolerance classes — fine (F), medium (M), coarse (C) and very coarse (V) — based on the nominal dimension range. For most custom sheet metal enclosures, ISO 2768-m (medium) is the sensible default.
The standard covers three categories of tolerance: linear dimensions, angular dimensions, and radii / chamfers. Below is the practical ISO 2768-m table for the linear dimensions you'll see on sheet metal parts.
| Dimension Range (mm) | ISO 2768-m Tolerance |
|---|---|
| 0.5 – 3 | ±0.1 mm |
| >3 – 6 | ±0.1 mm |
| >6 – 30 | ±0.2 mm |
| >30 – 120 | ±0.3 mm |
| >120 – 400 | ±0.5 mm |
| >400 – 1000 | ±0.8 mm |
| >1000 – 2000 | ±1.2 mm |
For angular dimensions on sheet metal, ISO 2768-m gives ±0.5° for dimensions up to 10 mm and ±1° above. If a bend or weld angle needs to be tighter than that, it must be individually toleranced on the drawing — and that tighter tolerance should match a real functional need.
Traditional vs GD&T Tolerancing
Traditional tolerancing — "100 ±0.1 mm" — treats every dimension as an independent linear tolerance. It works, but it stacks. On a part with five critical dimensions, the worst-case stack-up is five times the individual tolerance; the statistical stack-up is closer to the square root of the sum of squares, but in a tolerance chain that affects assembly fit, worst-case is what bites you.
GD&T — Geometric Dimensioning and Tolerancing, defined by ASME Y14.5 and ISO 1101 — replaces independent linear tolerances with feature control frames that describe the geometric relationship between features. The big win on sheet metal is that you can lock down the features that matter to assembly fit and let everything else float within a profile tolerance, which the fabrication process can hold without special effort.
The GD&T callats that pay off most on sheet metal enclosures are:
- Position (⊕) — replaces ±X mm on hole locations with a position tolerance referenced to a datum. A position tolerance of ±0.2 mm at MMC (maximum material condition) on four mounting holes is easier to manufacture than four independent linear tolerances. The same principle is what makes a hole pattern hold over a 42U assembly — see our 19 inch rack dimensions guide.
- Profile of a surface (⌒) — controls the shape of a curved or flat surface within a tolerance zone; ideal for sealing faces and gasket surfaces.
- Flatness (▱) — controls how flat a referenced face needs to be; critical for panels that mate to other parts or for gasket sealing.
- Concentricity / runout (◎ / ↗) — used on punched or laser holes that need to align with a mating feature.
If your part needs true 3D tolerancing with datum references — for instance, an enclosure that bolts to a mating panel and needs the holes to be co-planar with a sealing face — use GD&T. If your part is a simple flat panel with a few holes, traditional ISO 2768-m tolerancing is plenty.
Cost vs Precision: When Tight Tolerance Pays
The single biggest lever on sheet metal cost is over-tolerancing. A small mounting flange dimensioned at ±0.05 mm instead of ±0.2 mm will often force the shop to use slower cutting, secondary inspection, or hand correction. None of that affects the function of a cosmetic surface, but it all shows up on the invoice.
The rule of thumb is straightforward: tight tolerances only where the assembly actually needs them. Functional mating features — bolt patterns that mate with a motor, sealing surfaces that mate with a cover — earn it. Cosmetic surfaces, secondary holes, and dimensions that exist only to document the geometry do not.
A common mistake is to copy a drawing from a high-precision machined part and apply it to a sheet metal part. A CNC-milled bracket might need ±0.05 mm on every hole because it mates with a precision gearbox; a sheet metal enclosure door that simply closes over the bracket has no such requirement, and inheriting the precision specs is wasted money.
How to Specify Tolerances on a Drawing
For most custom sheet metal enclosures, the practical tolerance specification on a 2D drawing looks like this:
- Title block: "General tolerances per ISO 2768-m unless otherwise specified." That single line is your default.
- Critical features: individually dimensioned with linear or GD&T tolerances — bolt patterns, sealing faces, mounting holes that mate with another part.
- Notes: any process-critical requirements called out in plain language — "weld perpendicular to bend," "flatness of sealing face 0.3 mm per 300 mm," "bend radius R = 2 mm ±0.2 mm."
- Material and finish: specified separately, often with reference to internal standards (e.g. "cold-rolled steel DC01, 2 mm ±0.1 mm, powder coat RAL 7035").
That combination is enough for most sheet metal parts. Avoid: ± tolerances on every dimension, tolerances tighter than the process can hold, and tolerances that exist "just for documentation." Each one slows the quote, raises the price, or both.
Conclusion
Sheet metal tolerance is about asking for the precision the assembly actually needs, in the language the fabricator can hold without special effort. Default to ISO 2768-m, tighten only where function demands it, and use GD&T position and flatness callouts when the assembly fit depends on a geometric relationship rather than a single linear dimension. The result is a drawing that quotes faster, builds faster, and ships at a price that reflects the part's function rather than its appearance.
Send us your drawings and our engineers will review them for over-tolerancing before quoting — we routinely find 5–10 dimensions that can be loosened to ISO 2768-m with no impact on assembly fit, and that often drops unit price by 10–20% before production starts.