Sheet metal design comes down to a handful of rules that follow from how the process works: one uniform thickness for the whole part, an inside bend radius at least equal to material thickness, holes and features kept at least about two and a half times thickness away from any bend, a relief cut wherever a bend ends at an edge, and looser tolerances than you would expect from machining. Respect those and a fabricator can quote your part quickly and hit it consistently. Ignore them and you get either a rejected file or a part that is out of shape.

Why sheet metal is the cheap route to a metal enclosure

Laser cutting and press brake forming need no part-specific tooling. That means a one-off costs a fraction of what a machined or cast equivalent does, and a design change is a new flat pattern rather than a new tool. For enclosures, chassis, brackets, and panels, sheet metal is usually the most economical way to get a strong, EMI-shielding, professional-looking metal structure at low and medium volume — a point we make in our guide to choosing a process by volume.

Material choice drives most of the cost and behavior. Cold-rolled steel is cheap and strong but needs finishing to resist corrosion. Aluminum is light and easy to form and anodize but softer and more prone to cracking at tight bends. Stainless resists corrosion beautifully, costs more, and work-hardens as you form it. The tradeoffs are covered in aluminum vs steel.

Rule one: uniform thickness

A sheet metal part is made from one sheet. It has exactly one thickness everywhere, and no amount of CAD wishing changes that. If part of your design needs to be thicker, that region becomes a separate piece — welded, riveted, or fastened on.

Design to standard gauges rather than arbitrary numbers. Specifying a thickness that is not commonly stocked adds material cost and lead time for no benefit. Ask your fabricator what they keep in stock before you finalize the model.

Bend rules

  • Inside bend radius. Use at least one material thickness as the inside radius, and prefer the standard radii your shop's tooling already produces. A radius tighter than the material tolerates causes cracking on the outside of the bend, and aluminum is less forgiving here than steel.
  • One radius for the whole part. Every different bend radius may mean a different tool and another setup. Standardizing radii across the part is one of the easiest cost reductions available.
  • Minimum flange length. A flange has to be long enough for the press brake to grip and form — roughly four times material thickness plus the bend radius as a working minimum. Shorter flanges either cannot be formed or come out inaccurate.
  • Keep features away from bends. Holes, slots, and threads placed too close to a bend deform into ovals. Keep them at least about two and a half times material thickness from the bend line, measured from the edge of the feature.
  • Bend relief. Where a bend terminates at the edge of a face, add a relief notch at least as wide as the material thickness and slightly deeper than the bend radius. Without it, the metal tears at the corner of the bend.
  • Bend direction and sequence. The brake needs physical access. A box with four flanges bent up is trivial; a part with a flange folded inward over another flange may be impossible to form, regardless of how well it models. Sketch the forming sequence if the part is complex.
  • Countersinks and hems. A countersink deeper than roughly 60 percent of material thickness will distort. Hems and safety edges are a good way to stiffen a panel and remove a sharp edge without extra parts.

The flat pattern belongs to the fabricator

Bending stretches material along the neutral axis, so the flat blank is not simply the sum of the formed dimensions. The correction — bend allowance, bend deduction, or a K-factor — depends on the material, the thickness, the radius, and the specific tooling and machine.

Because of that, send the 3D formed part as your primary definition. Let the fabricator generate the flat pattern using their own numbers. Sending a flat DXF you calculated yourself invites parts that are the wrong size in a way nobody notices until assembly. Include a drawing with the dimensions that matter and the material spec, following the practice in what file formats to send a manufacturer.

Tolerances that suit the process

Sheet metal is not machining, and asking for machining tolerances on formed features raises price without improving anything.

  • Laser-cut features in the flat hold well — usually within a couple hundredths of a millimeter to a tenth, depending on thickness.
  • Formed dimensions across a bend are looser, typically several tenths of a millimeter, and stack up quickly across multiple bends.
  • Bend angles typically hold within about a degree, sometimes better with careful setup.

Dimension from a single flat face or a datum hole rather than chaining dimensions across bends, and where a precise relationship matters — a bearing seat, a connector cutout, mounting hole spacing — keep those features on one face so they are cut in the flat and never crossed by a bend. Where a tight fit is unavoidable, machine the feature after forming or use adjustable slots. The tolerancing discipline in GD&T basics applies directly.

Hardware, joining, and finishing

  • Self-clinching hardware — press-in nuts, studs, and standoffs give you strong threads in thin material and are the standard way to build a serviceable enclosure. Check the minimum thickness and edge distance the hardware specifies.
  • Tapping thin sheet rarely gives enough thread engagement. Use clinch nuts or an extruded and tapped hole instead.
  • Welding is strong and permanent but adds heat distortion and grinding labor. Spot welding is cheap on steel; TIG on aluminum needs more skill and cost.
  • Rivets and tabs assemble quickly with no heat. Self-locating tab-and-slot features double as assembly fixtures and are nearly free to add.
  • Finishing is where surfaces get their look and their corrosion protection: powder coating for durable color on steel and aluminum, anodizing for aluminum, plating and passivation for steel and stainless. Decide finishing early, because it affects hole sizes, masking, and grounding paths.

What drives the price

Roughly in order: material and thickness, cut path length, number of bends and setups, hardware count, secondary operations such as welding and tapping, finishing, and quantity. Fewer bends, fewer unique radii, fewer setups, and fewer secondary operations is the whole cost-reduction playbook, and it is the same thinking as general design for manufacturing.

Before you release for fabrication

Send the model to your fabricator for a DFM review before you commit. A good shop will tell you which radius to standardize on, which flange is too short, and which bend cannot be reached — usually within a day and at no cost, because it saves them work too. That review is one of the cheapest quality steps in the whole project. For how sheet metal fits alongside other options, see the manufacturing technologies pillar and our guide to finding a manufacturer.

Have a sheet metal enclosure or bracket that needs a manufacturable design? Send us the concept through our contact form and we will review it for formability, tolerances, and cost before anything is cut.