Tolerance and Surface Finish

Sheet metal tolerance is not one number. Cutting, forming, welding and finishing each control different features to different limits, and those limits are not equally tight. This page sets out which process owns which dimension, what the limits actually are, and how coatings and material move your numbers after the part is made.

Which Process Controls Which Dimension

When a dimension is out of tolerance, the first question is which operation created it. The answer determines whether the fix belongs in the drawing, the flat pattern, the fixture or a machining operation.

Feature	Controlled By	Achievable	Main Limiters
Cut profile / outline	Laser cutting	±0.05mm	Thickness, cut length, heat input, machine calibration
Hole diameter	Laser cutting	±0.05mm	Kerf variation with thickness; small holes less accurate
Hole position	Laser cutting + sheet flatness	±0.1mm	Clamping distortion, thermal relaxation, residual stress release
Bend angle	Press brake	±1°	Material spring-back, tool condition, operator over-bend
Flange length	Flat pattern calculation	±0.5mm	K-factor assumption, bend deduction convention
Flatness after forming	Bending sequence	Per review	Part stiffness, spring-back, fixturing during bending
Flatness after welding	Weld sequence and restraint	Per review	Weld shrinkage, heat input, part stiffness
Sealing face flatness	Final machining	Machined to spec	Requires a machining operation after forming or welding

Rule of thumb: if a tolerance is tighter than about ±0.1mm on a formed feature, forming will not deliver it reliably. The options are to machine it after forming, or to redesign the feature so forming error does not matter.

Building a Realistic Tolerance Stack

A sheet metal part passes through several operations and each one adds variation. The finished part carries all of them. The most common contributors on a bent, finished panel:

Contributor	Typical Contribution	Reducible By
Material thickness variation	±5% of nominal on mill sheet	Specifying a thickness tolerance class on the drawing
Cut profile position	±0.05mm	Little — this is close to the process limit
Flat pattern calculation	±0.2 to 0.5mm per bend	Stating the K-factor; simpler single-bend geometry
Spring-back variation	±0.5° to 1° per bend	Material control, tighter incoming specification
Coating buildup	+0.06 to 0.12mm per side	Thinner film, or machining after finishing
Weld shrinkage	0.3 to 1.5mm on a welded assembly	Design stiffness, sequence, or machining the critical face

For a fit-critical feature, the sensible approach is to stop stacking at the operation that can actually control it: specify machining after forming or finishing, and dimension that feature from the machined surfaces rather than from the raw part.

How Coatings Move Dimensions

Finish	Typical Build per Side	Dimensional Effect
Powder coating	60–120 µm	Adds material; also rounds sharp edges slightly
E-coating	15–25 µm	Minimal; the most dimensionally stable coating
Hot-dip galvanizing	60–100 µm plus process allowance	Largest effect; threads and close fits need allowance or masking
Anodizing (aluminium)	5–25 µm	Small but grows the part; dielectric, so it cannot be conductive
Passivation	Negligible	No dimensional effect; surface treatment only
Brushing / polishing	Material removed	Slightly reduces dimension; nominal is the finished size

Declaring Flatness So Both Sides Agree

Flatness without a measurement condition is not a requirement — it is a disagreement waiting to happen. Three things must be stated:

• Which faces — flatness of the whole part, or a named surface such as a gasket land.
• Over what length — flatness over 200mm and over 1000mm are very different requirements.
• Support condition — supported at two points, supported fully, or free. A thin panel measured unsupported will never meet a figure derived from a supported part.

Where flatness is functionally important — a sealing face, a gasket land, a heat-sink interface — the reliable route is to machine it after forming or welding. That adds an operation, and it is much cheaper to know at quotation than to discover on the first article.

Surface Finish: What to Specify

Surface State	Typical Ra	How to Specify It
As-cut laser edge	Ra 3–6 µm	Standard; no callout needed unless a heat-tint band is unacceptable
Deburred / edge broken	Ra 1–3 µm on the edge	Standard on all edges
Ground or machined face	Ra 0.8–1.6 µm	State the face, the Ra value and any flatness requirement
Brushed stainless	Ra 0.5–1.6 µm	Specify grain direction and which side is cosmetic
Powder coated	Not measured as Ra	Specify colour standard, coverage and thickness range, plus which face is visible
Sealing face	As-machined	State flatness, Ra and whether any edge break is permitted on that face

Mark the cosmetic side. On any visible part, mark both views with the cosmetic face and, for brushed or grain-finished surfaces, the grain direction. Without it the finish can arrive on the wrong side and the part is scrap — not because the finish is wrong, but because it is on the wrong face.

Datum Strategy for Sheet Metal Parts

Sheet metal parts are thin, flexible and often slightly warped after forming, which makes datum choice harder than it looks. A large flat machined face is not available on a folded panel, so the datum is usually an edge or a locating hole.

Situation	Recommended Datum	Reason
Flat panel, no forming	Two wide faces, opposed, with an edge as secondary	Standard; the faces are stable on a flat part
Bent panel	A locating hole plus a flange edge	The only repeatable features on a formed part
Feature must stay round after forming	Machine it after forming and datum from machined features	Forming error otherwise moves the datum
Welded assembly	Locating holes on the flat panel plus machined faces	Warpage makes a formed edge an unreliable datum

Common Mistakes

#	Mistake	Consequence	Correct Approach
1	Flatness specified with no measurement condition	Endless dispute; both parties technically correct	State faces, length and support condition.
2	Fit dimensions given before the coating is specified	Part does not fit after finishing	Specify the coating, then allow for build-up; or finish then machine.
3	Tight tolerance on a hole that gets bent	Oval hole; the fastener no longer seats properly	Move the operation after forming, or dimension generously.
4	Tolerance carried from thin to thick material unchanged	Unachievable; parts rejected	Widen the tolerance with thickness, or change material.
5	Relying on the general tolerance block for hole position	Position error accepted that should have been controlled	Call out hole position explicitly on features that matter.
6	Sealing face with a standard edge break applied	The gasket will not seal	Mark the sealing face and state no deburr, or a specified one.
7	Galvanized part with threaded holes not masked	Threads no longer fit their fasteners	Mask the threads, or oversize and re-tap after galvanizing.
8	Cosmetic face not marked	Finish on the wrong side; part is scrap	Mark both views, including grain direction.

Related Sheet Metal Pages

• Design for Sheet Metal — the geometry rules behind these tolerances
• Bend Radius and Bend Allowance — flat pattern accuracy and spring-back
• Welding Distortion Control — flatness on welded assemblies
• Material Selection — spring-back and thickness tolerance by alloy