Sheet metal guide

Why sheet metal earns its place

Sheet metal starts as flat stock of constant thickness, is cut to a developed pattern, and is then bent to shape. Because the material never changes thickness and the tooling only has to bend rather than melt or cut away bulk, the process is fast, cheap at low volumes, and scales to large parts that no molding press could handle.

• Strength to weight. Folding a flat sheet into a three-dimensional section produces stiffness out of almost nothing, which is why chassis, brackets, and enclosures are made this way rather than machined from solid.
• Low tooling burden. Laser cutting and press braking need no part-specific tooling at all, so the first part costs almost the same as the hundredth.
• Speed of iteration. A design change is a change to a flat pattern and a bend sequence, not a new tool.
• Size. A part measured in meters is routine, where the equivalent molded or machined part would be impossible or absurd.
• Material efficiency. Offcuts are recyclable and nesting software packs patterns tightly across the sheet.
• Finish flexibility. The same part can be powder coated, plated, anodised, brushed, or left raw without changing the tooling.

The constraint that governs everything is equally simple. You can cut and you can bend, but you cannot sculpt. A geometry that would be trivial to machine may be impossible to form, and the usual remedy is to split it into two parts and join them.

Flat patterns and bend allowance

A formed part exists in two states: the finished three-dimensional shape, and the flat blank it was cut from. Converting between them is the single most important calculation in sheet metal design, and getting it wrong produces a part that is dimensionally correct in CAD and the wrong size in reality.

When a sheet is bent, the outer surface stretches and the inner surface compresses. Somewhere between them lies a surface whose length does not change, called the neutral axis. The length of the neutral axis through the bend region is the bend allowance, and it is what the flat pattern must account for. Bend deduction expresses the same relationship from the other direction, describing how much shorter the flat blank is than the sum of the finished flange lengths.

The k-factor

The neutral axis does not sit at the middle of the sheet. Under bending it migrates toward the inner surface, and how far it migrates depends on the material, its temper, the bend radius, and the thickness. The k-factor expresses the position of the neutral axis as a fraction of the material thickness measured from the inner surface. It typically falls somewhere between roughly 0.3 and 0.5, with tighter bend radii pushing it lower.

The practical consequence is that a flat pattern is only correct for the k-factor, tooling, and material it was developed against. This is the reason to send a three-dimensional model rather than your own flat pattern: a blank developed against different assumptions will produce a part that is the wrong size once it is formed. If you have an existing flat pattern from a previous supplier, send it as reference alongside the 3D model, never instead of it.

Springback, and why bend angles vary

Metal bent past its yield point does not stay exactly where the tool leaves it. Some elastic deformation recovers when pressure is released, so the part springs back by a small angle. A brake operator compensates by overbending, but the amount of springback is not a constant. It varies with material, temper, thickness, and bend radius.

Thickness variation within the stock itself is the part designers most often overlook. Sheet is supplied to a gauge with a permitted range, not a single value. Twelve gauge steel, for instance, has a nominal thickness of about 0.1046 inches but is permitted to arrive anywhere between roughly 0.0986 and 0.1106 inches. Bending the two extremes of that range in the same tool with the same setup produces measurably different finished angles.

That 0.27 degree spread consumes more than half of a typical half-degree bend tolerance before any other source of error is considered. The lesson is not that tight bend tolerances are impossible, but that they must be specified deliberately, on the few angles that matter, with the knowledge that material variability alone will eat much of the budget.

• Tolerance stacks across bends. A dimension crossing three bends inherits the variation of all three.
• Dimension from cut edges wherever accuracy matters, because laser-cut features hold far tighter tolerance than formed ones.
• State which dimensions are critical so the bend sequence can be planned to favor them.
• Design clearance into mating interfaces rather than tightening a tolerance on a formed feature.

Bend radius

There is no universal minimum bend radius, and any single number offered as one should be treated with suspicion. The achievable minimum depends on the material and its temper, the thickness, whether the stock is hot or cold rolled, the forming method, and the tooling actually available on the brake.

The general principle holds regardless: the inside bend radius should be at least equal to the material thickness. Bending tighter than the material tolerates cracks the outer surface, and the harder or thicker the material, the larger the radius it demands. Ductile materials such as 5052-H32 aluminum form well at a radius equal to thickness or greater; harder tempers and thicker plate need several multiples.

These are approximate starting points for early design work, not specifications. Confirm against the material datasheet and against the tooling your supplier actually has before committing. One further habit saves a great deal of cost: use the same inside radius for every bend on the part wherever the design allows, because each different radius means a different punch and another setup.

Bend relief and tearing

Where a bend line ends part-way across a sheet rather than running clean off the edge, the material at the end of the bend is pulled in two directions at once. It will tear, and the tear will propagate. The remedy is bend relief: a small slot or notch cut at each end of the bend line so the forming and non-forming regions are separated before any force is applied.

• Make the relief at least as wide as the material thickness, and at least as deep as the bend radius plus the thickness.
• Round the end of the relief cut. A square internal corner is a stress concentration and a crack initiation site.
• Where two bends meet at a corner, relieve the corner rather than allowing the two forming zones to collide. A corner rip or a rounded corner relief both work; which is appropriate depends on whether the corner will later be welded.
• Bend lines running parallel to the material grain crack more readily than those running across it. On cosmetic or highly stressed parts, specify grain direction on the drawing.

Placing holes, slots, notches, and tabs

Every cut feature near a bend is at risk of distortion, because the metal in the bend region moves. Features cut before forming, which is the normal sequence, must therefore be positioned far enough away that forming does not pull them out of shape.

Where a feature genuinely has to sit closer to a bend than these guidelines allow, the alternative is to cut it after forming as a secondary operation. That holds position accurately and costs more, which is the right trade for a critical locating feature and the wrong one for a clearance hole.

Stiffening features

A flat panel is not stiff. Rather than moving to thicker and heavier stock, form stiffness into the part.

• Beads and ribs. A shallow formed channel running across a panel raises its bending stiffness substantially at no weight cost. Keep bead depth modest relative to thickness and give generous radii at each end.
• Flanges. Turning a short lip along a free edge is the cheapest stiffness available and also removes a sharp edge.
• Gussets. A formed or welded triangular web supporting a bend resists the flange folding open under load.
• Embosses and dimples. Localised forming that stiffens an area or provides a standoff without additional parts.
• Hems. Folding an edge back on itself doubles thickness locally, stiffens the edge, and makes it safe to handle.

Corners, jogs, and joining

Corners

Where two bends meet, the material has nowhere to go. A corner rip, which is a relief cut at the intersection, is the standard answer. It leaves a small gap at the corner, which matters for two reasons: a formed enclosure is never sealed as it comes off the brake, and the gap is visible on a cosmetic part. If the corner must be closed, plan for welding and dressing, or for a gasket compressed against a flange, and decide this before the flat pattern is fixed.

Jogs and offsets

A jog is a pair of opposing bends producing a small step, used where two panels must overlap while remaining flush. Keep the offset distance at least a few multiples of material thickness; below that the two bend regions interfere and the step forms inconsistently. Where a very small offset is genuinely required, machining or a dedicated jog tool is the honest answer rather than a press brake.

Joining

• Self-clinching hardware, the PEM-style nuts, studs, and standoffs, pressed into the sheet. The normal choice for enclosures and chassis. Specify the part number and the side it installs from, since that dictates the forming sequence.
• Weld nuts and weld studs where loads exceed what clinched hardware supports.
• Rivets and rivet nuts for thin stock and dissimilar materials.
• TIG, MIG, and spot welding for structural joins. Welding distorts locally, so specify which dimensions must be held after welding rather than before.
• Tab and slot features that locate two parts to each other before welding, which removes the need for a fixture and improves repeatability.

Drawing and dimensioning practice

How a sheet metal part is dimensioned decides whether it can be inspected and whether the tolerances mean anything.

• Dimension to virtual intersections, the theoretical point where two flange faces would meet if extended, rather than to the tangent of the bend radius. A virtual intersection dimension is invariant to the actual bend radius achieved, so it remains meaningful even if the radius shifts slightly.
• Send a 3D model as the master. Supply a flat pattern only as reference, and say which k-factor it was developed against.
• DXF exports should contain the cut profile on its own layer, with bend lines on a separate layer and no construction geometry. Duplicate and overlapping entities cause real problems in nesting and cutting.
• State material, thickness, and temper explicitly. "Aluminum" is not a specification; 5052-H32 is.
• Call out grain direction where bends are tight or the finish is cosmetic.
• Specify the finish, and state which faces are cosmetic. Coatings add thickness, so a tight hole that passed as-cut can fail after plating.
• Note hardware by part number and installation side.
• Say whether deburring is required and how sharp edges should be treated.

Materials in common use

A short pre-release checklist

• Every inside bend radius is at least material thickness, and the same radius is used throughout wherever possible.
• Bend relief is present at every bend that terminates within the sheet, with rounded ends.
• Holes sit at least 2.5 thicknesses from any bend, and 2 thicknesses from any edge.
• Slots are wider than the material, 2 thicknesses from edges, and 4 thicknesses from bends.
• Critical dimensions are taken from cut edges, or to virtual intersections, rather than across multiple bends.
• Corner treatment is decided, and sealing requirements are stated if the part is an enclosure.
• Material, thickness, temper, grain direction, and finish are all on the drawing.
• Hardware is called out by part number with the installation side noted.
• A 3D model is supplied as the master, with any flat pattern marked as reference only.