A folded part gets drawn twice: once as the shape the client sees, and once as the flat blank the cutter receives. Those two drawings are not the same size, and the difference is not a rounding error. On a sign tray or a fit-out reveal it is a few millimetres per bend, enough to turn a tight shadow gap into a visible one. Everything below is what I check before a flat pattern leaves my desk.
The flat blank is not the sum of the sides
When sheet goes round a bend, the outside stretches and the inside compresses. Somewhere through the thickness there is a fibre that does neither, and where it sits is what the K-factor describes: a number between 0 and 0.5, with 0.5 at mid-thickness. Air-bent mild steel usually lands near 0.41. Sharp bends pull it down towards 0.33, generous radii push it up towards 0.45. The bend allowance is the arc length along that fibre, and the flat length is the sum of the straight sections plus one bend allowance per bend.
The practical consequence is that two people can model the same bracket and produce flats that differ by millimetres, because their CAD sheet metal settings disagree. The fix is dull and it works: model the formed part, let the software unfold it, and set the K-factor to the value used by the shop that will actually bend it. I ask for their bend deduction table before I draw anything. A fabricator who bends every day has one for their own tooling and their own material, and it beats any published formula. And if the flat and the formed part ever disagree, the shop needs to be told which one is the master.
The die chooses your radius and your shortest flange
Two numbers a designer does not get to set freely. In air bending, both follow from the V-die opening, and the die follows from the thickness, roughly six to eight times it.
The inside radius comes out near one sixth of the die opening. A 2 mm part on a 12 mm die lands close to a 2 mm inside radius whether the model says 2 mm or a sharp corner. So model a radius of at least one material thickness. A sharp corner in CAD is a promise the brake cannot keep, and every downstream dimension inherits the mismatch.
The minimum flange is the harder constraint. Below roughly two thirds of the die opening the blank no longer rests on both shoulders of the die: it drops in, the angle goes wrong and the face marks.
| Thickness | Typical V-die | Shortest flange worth asking for |
|---|---|---|
| 1.0 mm | 8 mm | about 6 mm |
| 1.5 mm | 12 mm | about 8 mm |
| 2.0 mm | 12 to 16 mm | 8 to 11 mm |
| 3.0 mm | 20 to 25 mm | 13 to 17 mm |
| 4.0 mm | 25 to 32 mm | 17 to 21 mm |
| 5.0 mm | 32 to 40 mm | 21 to 27 mm |
If a detail calls for a 5 mm return on 2 mm aluminium, that is not a bending job. It is thinner material, a machined or extruded section, or a welded corner, and it is cheaper to decide that in CAD than on the shop floor.
Where the material fights back
Grade matters more than thickness here. Cold-rolled mild steel takes an inside radius of about one thickness. Stainless work-hardens and wants more, around one and a half thicknesses in 304 and two in 316. Soft aluminium in the 1050 and 5251 family behaves roughly like mild steel; the harder structural grades such as 6082 want two to three thicknesses and will crack at anything tighter.
Grain direction is the trap. Rolled sheet has a grain, and a bend line running across it is far safer than one running along it: bent parallel to the grain, the same material may need an inside radius fifty to a hundred per cent larger before it stops cracking on the outside face. On a part with bends in two directions, one of them is the parallel one, so either open its radius or accept that this is the bend that will craze.
Two more that show up at the wrong moment. Aluminium springs back more than mild steel, so on anything with a tight angular tolerance it is worth paying for a first-off sample bend rather than arguing about the batch. And tonnage scales: aluminium needs roughly half the force of structural steel, stainless roughly 1.7 times, which is why a three metre bend in 3 mm steel quietly rules out a small brake and changes who can make the part.
Pre-finished material deserves its own line. A tight radius cracks powder coat and crazes a laminate. Where the finish has to be perfect, bend first and coat after, and say so on the drawing.
Holes, reliefs and corners
Holes near a bend go oblong, because the material in the bend zone moves. Keep the edge of any hole, slot or notch at least one and a half thicknesses plus the inside radius away from the bend tangent. Closer than that and the part has to be bent first and drilled after: a second operation, a second setup and a line on the quote.
Where two bend lines meet, the corner needs a relief notch of at least one material thickness in each direction, or the material tears at the junction and the second bend fights the first. CAD sheet metal tools add these automatically when the feature tree is set up properly, and omit them entirely when someone has drawn the flat by hand.
For a tray, the corner detail is a real decision, not a default. A folded tab lapping over the adjacent return is quick and needs no welding, but on a painted or anodised face the lap telegraphs and the joint line catches dirt. A corner that is welded and dressed costs more and reads as a single piece, which is usually what a shopfront tray is being paid for.
What the brake can physically reach
Past two bends, sequence starts to constrain shape. Every flange already formed is an obstacle for the next stroke, so deep trays, returns that fold back on themselves and bends running in opposite directions on the same flange can all turn out impossible in the order they seem to want. Offline programming catches the collision before the job reaches the machine, but only if someone runs it, and the answer at that point is a redesign under time pressure. Short bends on a long brake are the other quiet one: a 60 mm bend on a three metre machine has to be centred carefully or it comes out of square. All of it is worth one question at quote stage, which is whether the part can be bent in the order it has been drawn, and on what tooling.
What to send, and what to expect back
Send the formed part in 3D, a dimensioned drawing of the formed part, and the flat only when it has been asked for. State which file is the master. Dimension from one datum face rather than chaining feature to feature, because a chain hands the shop your tolerance stack instead of your intent.
What a well set up brake holds, as a working assumption: bend angle to about half a degree, a dimension from the datum to a bend line to about 0.25 mm, and overall formed length to about 0.5 mm. Those numbers are comfortable on their own and less comfortable in fours. A tray with four bends between two visible edges can absorb a full millimetre of drift, which a 5 mm shadow gap will show and a butt joint between two trays will show twice. Decide which dimension the eye will judge, tighten that one, and open the rest.
The short version, and the order I work in: model the formed part, use the fabricator's K-factor, let the die set the radius and the minimum flange, keep holes and reliefs clear of the bend zone, check the sequence is buildable, and spend the tolerance where someone will look. Drawings that do this come back as parts that fit. Drawings that do not come back as questions on the day of installation, which is the most expensive day to answer them. That check is part of what I do on a production support job, before anything is cut.
