Good sheet metal design keeps the part buildable on a standard press brake with standard tooling: one material thickness, an inside bend radius at least about equal to the thickness (more for hard alloys), reliefs where bends meet edges, holes kept away from edges and bends, and flanges long enough to sit across the die. Break those rules and parts crack, holes distort, or the bend simply cannot be made.
Key points
- Design the whole part in one thickness. Sheet comes in one gauge per part.
- Use an inside bend radius of at least about the material thickness, and the same radius for every bend.
- Add bend reliefs where a bend runs into an unbent edge, and corner reliefs where bends meet.
- Keep holes at least about 2 × thickness from edges and about 2.5 × thickness plus the radius from bends.
- Make flanges at least about 4 × thickness long, or whatever the shop’s die needs.
- Every bend is a press brake operation. Fewer bends, all in the same direction, cost less.
How is a sheet metal part made?
Most sheet metal parts start as a flat pattern cut from a sheet, usually by laser cutting, punching or waterjet. The flat blank is then bent on a press brake, one bend at a time, by pressing it with a punch into a V-shaped die.
That sequence explains every rule below. The flat pattern must be unfoldable from one sheet. Each bend must be reachable by the punch without the part hitting the machine. And metal stretches on the outside of a bend and compresses on the inside, which moves holes and edges that sit too close. The sheet metal fabrication cost guide explains how cutting, bending and finishing add up into a price.
Design rules at a glance
These are widely used rules of thumb, with T for material thickness and R for inside bend radius. Your fabricator’s tooling and material may allow less, or need more.
| Feature | Rule of thumb | Why |
|---|---|---|
| Material thickness | One thickness for the whole part | A part is cut from one sheet |
| Inside bend radius | At least about 1 × T for mild steel and soft aluminium; more for hard alloys | Tight radii crack the outside of the bend |
| Radius consistency | One radius for every bend | One tool setup instead of several |
| Bend relief width | At least about 1 × T | Lets the bend form without tearing |
| Bend relief depth | At least about R + T past the bend | Clears the full bend zone |
| Minimum flange length | At least about 4 × T, or what the die requires | The flange must span the V-die opening |
| Hole diameter | At least about 1 × T | Smaller holes are hard to punch and distort when cut |
| Hole to edge | At least about 2 × T | Prevents bulging and tearing at the edge |
| Hole to bend | At least about 2.5 × T + R | Prevents the hole stretching into an oval |
| Hole to hole | At least about 2 × T | Keeps the web between holes from distorting |
| Hems | Inside diameter at least about 1 × T for an open hem | A closed hem can crack thicker or harder sheet |
Bend radii: why tight bends crack
When sheet bends, the outside surface stretches. The tighter the radius, the more it stretches, and past a point it cracks. Soft materials such as mild steel and annealed aluminium tolerate an inside radius around the material thickness. Harder alloys and tempers need more, sometimes several times the thickness.
Bend direction relative to the sheet’s rolling direction matters too: bending across the grain is more forgiving than bending along it. For hard materials, note the grain direction on the drawing if it matters.
Use the radii your fabricator’s tooling actually produces. A radius that matches no punch and die either gets changed by the shop or needs special tooling.
Reliefs: giving the metal somewhere to go
Where a bend line runs into an unbent edge, the metal at the end of the bend is caught between bent and flat material. Without a relief it tears or bulges. A bend relief is a small notch cut at the end of the bend line. Where two flanges meet at a corner, a corner relief stops them colliding and leaves a clean gap for welding or for the corner to stay open.
Reliefs are cut with the flat pattern, so they cost almost nothing. Forgetting them costs a remade part.
Holes, slots and edges
A hole near an edge bulges the edge as it is punched or as the part is bent. A hole near a bend is worse: the metal around it stretches with the bend and the hole goes oval. Keep holes back from bends by at least the rule in the table, or accept that they will be cut after bending, which adds an operation.
Small holes are a problem too. A punched hole smaller than about the material thickness is hard on the punch, and a laser-cut one in thick plate may show taper and heat effects. If a small hole needs a precise size, consider drilling or reaming it.
Flanges and bend sequence
A flange must be long enough to rest across the V-die while it is bent; a short flange falls into the die. The die opening grows with material thickness, so minimum flange length does too. A common rule of thumb is about four times the thickness, but the real limit is the shop’s die.
Bend sequence matters for boxes and channels. A deep, narrow U-channel can trap the punch: after the second bend, the part may hit the tool. Check that every bend can be made after the ones before it, or ask the fabricator early. Bends all in one direction mean less flipping of the part between operations.
Flat patterns and the K-factor
The flat pattern is longer than the inside dimensions and shorter than the outside ones, because the metal stretches outside the neutral axis and compresses inside it. The K-factor is where the neutral axis sits, as a fraction of thickness from the inside face. Typical values fall somewhere around 0.3 to 0.5. The bend allowance, the length of the neutral axis through the bend, is:
Bend allowance = (π ÷ 180) × bend angle in degrees × (R + K × T)
Worked example: unfolding an L-bracket and checking it against the rules. K = 0.44 is an example value.
2 mm mild steel, inside radius 2 mm, one 90° bend, outside flange lengths 40 mm and 30 mm, a hole in each flange.
| Line | Calculation | Result |
|---|---|---|
| Bend allowance | (π ÷ 180) × 90 × (2 + 0.44 × 2) = 1.5708 × 2.88 | 4.52 mm |
| Outside setback per flange | tan(45°) × (R + T) = 1 × (2 + 2) | 4.00 mm |
| Straight length, flange A | 40 - 4.00 | 36.00 mm |
| Straight length, flange B | 30 - 4.00 | 26.00 mm |
| Flat pattern length | 36.00 + 26.00 + 4.52 | 66.52 mm |
| Minimum flange | 4 × 2 mm | 8 mm: both flanges pass |
| Minimum hole to edge | 2 × 2 mm | 4 mm |
| Minimum hole to bend | 2.5 × 2 mm + 2 mm | 7 mm |
| Relief, if the bend meets an edge | width 1 × 2 mm, depth 2 + 2 mm | 2 mm wide, 4 mm deep |
A different K-factor changes the flat length, which is why the fabricator’s own value matters for parts with many bends: a small error per bend adds up across the part.
Nesting and material use
The flat pattern also sets how many parts fit on a sheet. Compact flat patterns with straight edges nest tightly; awkward shapes waste sheet. The nesting and material utilisation guide covers how a shop charges for the sheet, and the laser cutting cost guide covers the cutting time that each contour and pierce adds.
What to send for a quote
Send a 3D model in STEP so the fabricator can unfold it with their own K-factor and tooling, plus a DXF of the flat pattern if you have already unfolded it, and a drawing for bend directions, tolerances and finish. The STL vs STEP vs 3MF guide explains why a mesh is a poor input for sheet metal. Every rule in this article is part of design for manufacturing, and the sheet metal technology page covers the process itself.
Quotometry does not price bent sheet metal yet: it prices flat parts cut by laser, waterjet or plasma from a DXF or SVG drawing, but unfolding, bends and the checks above are not built.
Questions people ask
What is the minimum bend radius for sheet metal?
For mild steel and soft aluminium grades, an inside bend radius about equal to the material thickness is a common safe starting point. Harder alloys and tempers, such as 6061-T6 aluminium, crack at tight radii and need a larger one, often several times the thickness. Use the radii your fabricator's tooling actually produces, and keep one radius for every bend if you can.
Why does sheet metal need bend reliefs?
Where a bend line runs into an unbent edge, the material at the end of the bend has nowhere to go. Without a relief it tears or bulges. A small notch at the end of the bend, at least as wide as the material is thick and running a little past the bend, lets the bend form cleanly and keeps the corner tidy.
How close can a hole be to a bend?
A common rule is at least about 2.5 times the material thickness plus the bend radius, measured from the hole's edge to the bend. Closer than that, the hole stretches into an oval as the bend forms. If a hole must sit closer, it can be cut after bending, at extra cost, or the bend line can be relieved with a slot.
What is a K-factor and do I need to set it?
The K-factor gives the position of the neutral axis inside the bend as a fraction of the thickness. CAD software uses it to unfold a bent part into a flat pattern. Typical values sit somewhere around 0.3 to 0.5, depending on material, radius and tooling. If your fabricator gives you their value, use it, or send the bent model and let them unfold it.
Quotometry prices every part from your own machines and rates, on your website, in seconds.