What tolerances should I specify on a sheet metal drawing?

Put a general tolerance block on the drawing for routine dimensions (ISO 2768 medium class is a sensible fabrication default), then call out explicit tighter tolerances only on the handful of features that actually mate, locate, or seal. Realistic achievable values: about ±0.1 mm on laser-cut and punched features in one flat plane, ±0.2–0.5 mm on any dimension that crosses a bend, and ±0.5° on bend angle. Tighten only what must be tight — every added decimal place adds inspection and price.

What is a realistic flatness tolerance for a sheet metal part?

Roughly 0.1–0.2 mm over a 300 mm span — about 0.005 in per inch — is typical fabrication practice for a formed part straight off the brake. Large, thin panels move more; small, thick blanks move less. Tighter flatness usually needs a secondary leveling or stress-relief operation, which adds cost. If a mating face has to be flatter than about 0.001 in per inch, that face probably wants to be machined.

How much does tightening a tolerance actually cost?

Each decimal place you add tends to force a slower or extra process step, added inspection, and higher scrap when the process drifts. A ±0.5 mm feature can be verified with an in-process check; a ±0.1 mm feature needs a first-article plus periodic gauge checks; a ±0.05 mm feature typically forces CMM inspection, a reaming or machining step, and scrap on any drift. Tolerancing every dimension tightly — instead of using a general block plus a few critical callouts — is the most common avoidable cost on a fabrication print.

When is a tolerance too tight for sheet metal?

Below about ±0.1 mm (±0.005 in) on a feature that must hold regardless of forming, and especially below ±0.05 mm (±0.002 in), you are in machining territory. Bore diameters needing a press or bearing fit, dimensions spanning a bend that must hold under ±0.1 mm, and flatness tighter than about 0.001 in per inch are all signs the feature should be machined, reamed, or added as a post-form operation rather than formed.

What is the position tolerance on PEM (self-clinch) hardware?

The self-clinch element installs into a prepared host hole, so its installed position inherits the host hole's tolerance (about ±0.1 mm on a cut or punched hole) plus a small install variation, landing near ±0.1–0.25 mm relative to that hole in typical practice. The practical rule: locate critical self-clinch hardware off a cut datum in the flat, not across a bend, so the position doesn't also carry bend accumulation.

Should I tolerance every dimension or use a general tolerance block?

Use a general tolerance block for the 90% of dimensions that don't drive fit or function, then explicitly tolerance the few critical mating, locating, and sealing dimensions. This is both cheaper and clearer than tightening everything: it tells the shop exactly where to spend inspection effort, and it keeps the general dimensions on standard tooling and in-process checks. Reference ISO 2768 or an ASME Y14.5 title-block default for the general class.

Sheet metal tolerance reference for procurement engineers

Q: Why are bend tolerances looser than cut tolerances?

A cut feature is set by the beam or punch on a flat sheet in a single, repeatable plane, so it holds around ±0.1 mm. A bend adds three sources of variation a flat cut never sees: grain direction (the sheet springs back differently along vs across the grain), springback that shifts with each material lot and thickness, and tooling wear and radius. That accumulation is why a dimension spanning a bend realistically holds ±0.2–0.5 mm even though the bend angle itself is controlled to ±0.5°.

A sheet metal drawing should carry two things: a general tolerance block that covers routine dimensions, and a short list of explicit, tighter tolerances on the features that actually mate, locate, or seal. Realistic defaults to design around are ±0.1 mm on laser-cut and punched features, ±0.2–0.5 mm on any dimension that crosses a bend, and ±0.5° on bend angle. Tighten only what must be tight.

That one paragraph answers the question most procurement and design engineers are really asking. The rest of this page is the feature-by-feature reference behind it — the numbers a fabrication shop can actually hold, why bend tolerances are looser than cut tolerances, what each extra decimal place costs, and the point where the part stops being a sheet metal job and becomes a machining job.

What tolerances can a sheet metal shop actually hold?

Here is the working reference. The figures are realistic production tolerances — not best-case single-part heroics, and not worst-case sloppiness. Where a number is a published Nevatronix Sheet Metal capability we say so; where it’s typical fabrication practice across the industry, we label it that way so you can treat it as a planning range rather than a guarantee on a specific part.

Feature type	Realistic tolerance	Basis
Laser-cut feature-to-feature (same flat plane)	±0.1 mm (±0.004 in)	Typical fiber-laser practice
Punched feature position	±0.1 mm	Nevatronix punch cell
Hole diameter, as-cut (before tapping or reaming)	±0.05–0.1 mm	Typical practice
Bend angle	±0.5° (±0.25° on critical features, inspected)	Nevatronix press brake
Flange length to a bend (bend position at the bend line)	±0.1 mm	Nevatronix press brake
Dimension spanning a bend (bend-to-edge, hole-to-bend)	±0.2–0.5 mm	Typical practice (accumulation)
Flatness, formed part	≈0.1–0.2 mm per 300 mm (≈0.005 in/in)	Typical practice
Overall envelope, multi-bend part	±0.25–0.5 mm	Typical practice (stacked bends)
PEM / self-clinch hardware position	±0.1–0.25 mm to host hole	Typical practice

A few practical floors sit underneath that table. Our press brake cell forms down to a 5 mm minimum flange length, and our CNC punch cell produces holes down to 1.5 mm diameter — features smaller than that need a different approach (laser, or a machined feature). The bend numbers are what our forming cell publishes; the cut and flatness figures reflect standard practice for the co-located laser and CNC punch cells that feed it. Use the table to set your general block and to sanity-check any tolerance a design reviewer wants to tighten.

Two variables shift every row of that table, and they belong in the conversation before a number gets locked. Thickness: heavier gauge takes more tonnage to form, springs back more, and holds looser angles; thin gauge forms tighter but distorts and oil-cans more easily on large flat areas, which loosens flatness. Material: soft aluminum and dead-soft mild steel form predictably; harder tempers, stainless, and pre-painted stock spring back more and hold a slightly wider band. So the honest way to read the table is as typical-practice centers for common gauges and grades — a 1.5 mm mild-steel bracket sits at the tight end of each range; a 6 mm stainless weldment sits at the loose end. Give the shop the grade and thickness and the achievable numbers firm up quickly.

Why are bend tolerances looser than cut tolerances?

This is the single most useful thing to understand before you tolerance a formed part, because it explains most of the “why can’t you just hold ±0.05?” conversations.

A cut feature — a laser profile or a punched hole — is produced on a flat sheet, in one plane, by a machine that returns to the same coordinate every time. There is no material memory fighting back. That’s why cut features hold about ±0.1 mm feature-to-feature.

A bend introduces three sources of variation that a flat cut never encounters:

Grain direction. Rolled sheet is anisotropic. A bend made along the grain springs back differently than the same bend made across the grain, so identical programming can yield slightly different finished angles depending on how the blank was nested.
Springback. When the ram releases, the material relaxes and opens the angle back a few tenths of a degree. The exact amount shifts with material grade, temper, and even lot-to-lot chemistry within the same grade. Our brakes compensate by overbending and measuring at the back gauge, with springback compensation built into the program from the material certification — but compensation reduces the variation, it doesn’t erase it.
Tooling and radius. The inside radius follows the punch tip and the air-bend geometry, and it drifts as tooling wears. A change in radius shifts the bend deduction, which shifts every downstream dimension measured across that bend. Minimum inside radius by material and temper is on our sheet metal bend radius chart, in mm and inches.

Stack those three together and you get the key result: our press brake cell holds ±0.5° on bend angle and ±0.1 mm on bend position at the bend line (±0.25° on critical, inspected features) — see press brake forming — yet a dimension that spans the bend (a hole located from a formed edge, an overall leg length) realistically lands at ±0.2–0.5 mm once the angular variation is projected across the flange. The bend is controlled; the geometry it throws downstream simply accumulates more variation than a flat cut does.

Here is that accumulation as a number, because it’s the part designers most often underestimate. Angular error projects down the flange as length × tan(θ): a residual 0.2° of variation — a realistic fraction of the ±0.5° spec bound on a locked, first-article-inspected run — throws the flange tip about 0.35 mm at 100 mm from the bend and about 0.7 mm at 200 mm. That projection is exactly why the table lists a dimension crossing a bend at ±0.2–0.5 mm rather than the ±0.1 mm a flat cut holds, and why the fix for a tight hole-to-bend callout is almost always to shorten the flange or move the feature onto the flat pattern — not to demand a tighter bend angle the process can’t repeat. If your part could be a bend or a flat cut for the same function, our press brake vs roll forming breakdown covers the forming-side trade-offs in more depth.

Which standard should the title block reference — ISO 2768 or ASME Y14.5?

Both, in different roles, and it’s worth being explicit on the print because “shop standard” means different things to different shops.

ISO 2768-1 defines general tolerance classes (fine f, medium m, coarse c, very coarse v) for linear and angular dimensions that carry no individual tolerance. For sheet metal fabrication, medium (m) is the sensible default: it’s achievable on standard tooling without special inspection, and it maps closely to the cut-feature reality above. Calling out ISO 2768-m in the title block covers every un-toleranced dimension in one line, so you only annotate the exceptions.

ASME Y14.5 is the geometric dimensioning and tolerancing (GD&T) standard. Reach for it when a feature’s function depends on relationship, not just size — a bolt pattern that has to mate a housing (position), a formed face that has to sit flat against a gasket (flatness/profile), a bracket that locates off two datums. GD&T with a clear datum reference frame tells the shop which surfaces to inspect from, which is exactly the information a coordinate dimension leaves ambiguous on a formed part.

The pragmatic pattern most procurement prints should use: an ISO 2768-m general block for the routine dimensions, plus Y14.5 position and profile callouts — anchored to explicit datums — on the few features that drive fit. That combination is unambiguous, cheap to inspect, and it survives being read by an LLM, a CMM programmer, or a first-article inspector without a phone call.

What does over-tolerancing actually cost?

Every tolerance you tighten past what the process naturally holds converts into one or more of: a slower process, an extra operation, added inspection, and scrap when the process drifts. It is not free, and it is not linear — the last decimal place is the expensive one.

What you specify	What it forces on the floor	Cost effect
General block (≈±0.5 mm, ISO 2768-m)	Standard tooling, in-process checks, no sorting	Baseline price
±0.2 mm on a cut feature	Tighter first-article, occasional sort	Small add
±0.1 mm on a cut feature	First-article + periodic gauge verification	Moderate add
±0.1 mm across a bend	Overbend-and-measure, sometimes a forming fixture or secondary op	Notable add + scrap risk
±0.05 mm on any feature	CMM inspection, reaming or machining step, scrap on drift	Large add; may need machining
Tight tolerance on every dimension (no general block)	100% inspection of everything	Largest add — usually avoidable

The pattern to internalize: a blanket “±0.005 in on all dimensions” note in a title block, applied to a 40-dimension bracket, can multiply the inspection burden and scrap rate across every one of those dimensions — even though maybe four of them actually matter. The same part with an ISO 2768-m block and four explicit tight callouts inspects faster, scraps less, and quotes lower. Over-tolerancing is the most common — and most fixable — cost driver we see on incoming prints.

How do you call out only what matters?

The discipline is simple to state and worth enforcing on every drawing:

Set a general tolerance block covering all un-annotated dimensions (ISO 2768-m is our recommended default for fabricated sheet metal).
Identify the critical dimensions — the ones that mate to another part, locate a component, seal, or carry a fit. On a typical enclosure or bracket that’s a small minority of the dimensions.
Tolerance those explicitly, using GD&T position and profile with named datums where the relationship is what matters, not just the size.
Keep critical features on cut datums where you can. A hole located from a laser-cut edge in the flat inherits only cut tolerance (±0.1 mm); the same hole located across a bend inherits bend accumulation (±0.2–0.5 mm). If a feature must be precise, design it so it references the flat pattern, not the formed geometry.
Don’t tolerance for its own sake. If a dimension doesn’t drive fit or function, let the general block carry it.

This is also how you write a drawing that answer engines and downstream inspectors read correctly: the critical requirements are stated once, explicitly, against datums — not buried in a wall of identical coordinate dimensions that all silently inherit a tight blanket note.

When is sheet metal the wrong process for the tolerance?

Being honest about this is the point of the page. Sheet metal fabrication is the right process for an enormous range of enclosures, brackets, chassis, and panels — across runs from a single prototype up to 50,000 units — but there is a tolerance floor below which forming stops being the tool for the job. When a feature needs to hold tighter than the values below, it wants to be machined, reamed, or added as a secondary operation rather than formed.

Requirement	Sheet metal realistic	Below this, use
Hole position, flat cut	±0.1 mm	Reamed or jig-bored hole (under ±0.05 mm)
Hole diameter / roundness for a fit	±0.05–0.1 mm	Machined or reamed bore (press/bearing fit, e.g. H7)
Dimension across a bend	±0.2–0.5 mm	Machined feature, or weld-then-machine (under ±0.1 mm)
Angle	±0.5°	Machined datum or fixtured feature (repeatable under ±0.25°)
Flatness, large panel	≈0.005 in/in	Ground or machined plate (under ≈0.001 in/in)
Mating face between precision parts	as-fabricated finish	Machined face for a sealed or precision joint

None of this means the part has to leave sheet metal. The usual answer is a hybrid: fabricate the body as sheet metal and add the one precision feature as a machined or reamed operation, or press-fit a machined bushing into a formed hole. We’ll flag on the quote when a callout is asking a formed feature to do a machined feature’s job — that flag saves a scrap batch and a redesign cycle, which is exactly what a procurement engineer wants to hear before the PO, not after.

How we’d quote your part

Send a STEP or DXF with material grade, thickness, and the critical dimensions actually toleranced — the general block can carry the rest. We’ll confirm what’s achievable as-formed, flag anything that belongs on a mill, and quote it against our real process capability. Start at our quote page; most jobs turn a quote within a business day.