Sheet Metal Profile Builder

Any open chain: straight segments joined end to end by bends. L brackets, U and C channels, Z and offset profiles, hat sections, guards, covers, trim. What it deliberately cannot do is branch, close back on itself, or hold arbitrary sketch curves — that constraint is what keeps it fast to drive and exact to compute.

To whichever datum you choose, once, for the whole profile. Outside apex is the default and means the theoretical sharp corner where the outside faces would meet if extended past the radius — the datum most drawings use. You can also measure to the inside apex, or tangent to tangent for the straight material only. The formed view draws construction lines out to the exact corner each length runs to, so you can see the datum rather than take it on trust.

Each bend has its own outside, so on a profile whose bends alternate, consecutive corners sit on opposite physical faces. The arithmetic is unaffected — the setback at a corner depends only on that bend, not on which way it turns — but the meaning is worth seeing rather than reading, which is why the construction lines are drawn per bend. If your drawing dimensions a Z web differently, switch to the tangent basis and enter the straight material directly.

Bend direction is stated as seen from one face of the flat blank: the face that lies on the left of the run from the first segment onward. A bend is UP when it folds toward that face and DOWN when it folds away from it. This describes the part, not the machine — it does not mean the ram travels up or down.

Because a chain of bends is only useful if each one says which way it folds, and a layer is the least intrusive place to put that. Every bend centreline goes on exactly one of the two — nothing is duplicated onto a generic layer. The CUT layer holds the blank perimeter and nothing else: no text, no dimensions, no construction lines.

The angle bent through. 0° is flat stock, 90° is a square corner, 180° folds the two segments back against each other. The included angle between the segments is 180° minus that. The two readings happen to coincide at exactly 90°, which is why the ambiguity survives in so many places.

On the tangent basis, yes to both. On the apex bases a 180° bend is refused, because the faces are then parallel and there is no sharp corner left to measure to — that is a real property of the geometry rather than an arbitrary limit. Acute bends are fine on every basis; we do not copy the "90° or greater" restriction some CAD packages put on their tangent option, because our model has no reason for it.

Nothing in the geometry. It labels the part and travels into the DXF comment. It does not set a K-factor, a springback allowance or a minimum radius, because we have no press, no tooling data and no test coupons — any number attached to a material name here would be invented. K-factor and inside radius stay visible and are yours to set. One exception, in the rough press-brake check only: stainless uses its own published radius figure (about 0.21 × the die opening instead of 0.16) when it works out the die your radius needs.

A blank has two dimensions. Every number on the page — flat length, bend positions, allowances — is computed without a width, so the calculation works whether or not you give one. Rather than invent a width so the button can light up, the export stays off until you enter a real one.

The chain curls far enough that the material runs into itself, so the shape cannot be folded from one blank however you sequence it. The check looks at the real material outline including thickness, not just the centreline. It is a geometry check, not a manufacturability check: a profile can pass and still be impossible with a particular tool.

In air bending, about 0.7 times the V-die opening, measured to the outside of the bend — shorter and the flange drops into the die. The press-brake check under the results takes the wider of two dies: a typical one for your thickness from a published table (6 to 12 times the thickness), and the one that air-bends your inside radius (about the radius divided by 0.16 for mild steel, 0.21 for stainless). Each end flange is checked against the die its own bend needs; bends under 90° are judged as for 90°, which errs on the safe side. A narrower die allows a shorter flange but leaves a tighter radius. It is a rough guide from tooling makers’ figures; your own tooling decides.