Guides / Chassis / Design for Manufacture

Designing a Folded Sheet Cover That Fits and Looks Right

September 19, 2026

Sheet metal is the cheapest way to enclose a volume, and it follows a completely different set of rules from machining. A designer who draws a folded part the way they draw a milled part produces something that either cannot be made or arrives nothing like the model.

Bend radius and bend allowance

When sheet is bent, the outside stretches and the inside compresses. Somewhere between them is a neutral axis that does not change length. That is why the flat blank is not simply the sum of the finished dimensions.

Two things follow:

1. Specify the inside bend radius. A safe default is an inside radius equal to the material thickness. If you do not say, the shop picks tooling and your flat pattern is wrong.
2. Let the shop calculate the flat pattern. Send the 3D model and the finished dimensions, not your own unfolded blank. Bend allowance depends on the shop’s tooling, its material and its K-factor, and their number will be better than yours.

Dimension the part from the outside faces or from a datum face, not by chaining flange lengths. Chained dimensions turn every bend tolerance into an accumulated error.

The limits a press brake actually has

These are the constraints that cause redesigns:

• Minimum flange length. The flange has to be long enough to sit on the die. A rough rule is about four times material thickness plus the bend radius. Shorter flanges need special tooling or a different approach.
• Hole to bend distance. A hole too close to a bend distorts into an oval as the material moves. Keep holes at least two and a half times material thickness plus the bend radius away from the bend line, or add a relief cut.
• Bend relief. Where a bend stops partway along an edge, the material tears unless a relief notch is cut at each end. This is standard and the shop will usually add it, but it is a visible feature so you should decide its shape.
• Tool access. A box with four upstanding sides can become impossible to fold, because the last bend needs the press tooling to occupy space that the earlier bends now fill. This is the classic sheet metal surprise.
• Grain direction. Sheet has a rolling direction. Bending across the grain is safer, bending along it risks cracking on tight radii in harder alloys. On a cosmetic part, grain direction also affects how the surface finishes.

Tolerances you can actually expect

Press brake work is not machining and should not be toleranced as if it were.

Feature	Realistic tolerance
Flat blank dimensions (laser cut)	±0.1 to ±0.2 mm
Hole position in the flat	±0.1 mm
Bend angle	±0.5 to ±1 degree
Dimension across one bend	±0.2 to ±0.4 mm
Dimension across several bends	±0.5 mm or more, accumulating
Squareness of a folded box	0.5 to 1 mm over 300 mm is normal

A drawing that puts ±0.05 mm on a folded dimension will either be quoted with a machining operation added, or quoted by somebody who has not read it.

Designing so squareness does not matter

Since a folded box is not square, the design should not depend on it being square.

• Let the machined parts set the datums. A billet front and rear panel bolted into a folded sleeve define the geometry. The sleeve just has to get close.
• Use slotted holes where the folded part attaches to the machined part, so assembly can take up the error.
• Put the visible gap between a machined part and a machined part, not between two folded parts.
• Add a shadow gap or a step anywhere a folded edge meets a machined face, so the eye reads a line rather than a mismatch. See the panel gaps guide for the tolerance stack behind this.

Finish on sheet parts

Two points that surprise people:

• 5052 and 5754 anodize to a different tone from 6061 and 6063. A folded cover and a billet panel anodized black in the same tank will not match exactly. Bead blasting both to the same grit narrows the gap, and going darker narrows it further.
• The sheet surface is not a machined surface. Mill finish sheet carries its own texture and can show rolling marks after anodize. If appearance matters, specify the sheet surface quality or plan to blast it.

Cost levers

• Fewer bends. Each bend is a setup on the brake. A part with three bends is cheaper than one with seven, and a cover made from two simple parts can beat one complicated part.
• Nothing tighter than it needs to be. A general tolerance of ±0.3 mm on a cover with three critical features called out tighter prices far better than ±0.1 mm everywhere.
• Standard material thickness. 1.0, 1.5, 2.0 and 3.0 mm are stocked. 1.8 mm is a special order.
• Tabs and slots instead of brackets. Designing interlocking tabs into the flat pattern removes separate parts and assembly steps.
• Hardware inserts (PEM style) instead of tapped holes. You cannot usefully tap 1.5 mm sheet. A self clinching nut is the standard answer and it goes in at the press, cheaply.

Drawing checklist

• 3D model plus a dimensioned drawing of the finished part, not your own flat pattern
• Material, alloy, temper and thickness
• Inside bend radius, stated
• Dimensions from a datum face, not chained through flanges
• Bend angle tolerance separate from linear tolerance
• Hole to bend distances checked
• Bend reliefs shown, with their shape decided
• Hardware inserts called out by part number and shown on the correct face
• Which faces are cosmetic, and the finish
• Grain direction if it affects appearance or a tight bend

Frequently asked questions

Keep reading

• What an Amplifier Chassis Actually Costs to Manufacture
• Billet, Extrusion or Folded Sheet: Choosing How to Build a Chassis
• Specifying and Machining a Heatsink Extrusion for an Amplifier

This guide is part of Audio Chassis Manufacturing: The Whole Picture, one of four sections in the guide library.