Sheet-Metal Work From Design to Finished Part
Sheet parts are the cheapest way to make many industrial components — if they are designed properly. Bend radii, K-factor, hole-to-bend distance, flat patterns and the expensive mistakes.
Many parts that get carved out of a steel block could have been a cut and folded sheet — at a fifth of the price and a third of the time.
Sheet metal works when the part is essentially a plate bent in a few places: frames, covers, brackets, supports, panels.
The route a sheet part takes
- Cutting — laser, plasma, waterjet or punching
- Bending — on a press brake
- Finishing — tapping, riveting, welding, painting
Each stage has limits that have to be respected in the design.
Bend radius — the first thing to know
Sheet cannot be folded to a sharp corner. There is always an internal radius.
Rule of thumb: internal radius at least equal to material thickness.
| Thickness | Minimum internal radius (mild steel) |
|---|---|
| 1 mm | 1 mm |
| 2 mm | 2 mm |
| 3 mm | 3 mm |
| 5 mm | 5–8 mm |
For aluminium and stainless the number is larger — 6000-series aluminium may need twice the thickness or it cracks.
If you leave the bend radius at zero in CAD, the flat pattern comes out wrong and the finished part will not match your model.
K-factor, and why the flat length is not the sum of the sides
When sheet is bent, the outer surface stretches and the inner one compresses. Somewhere through the thickness, length does not change — the neutral axis.
The K-factor states where that axis sits as a fraction of thickness. For mild steel it is usually 0.33 to 0.45.
The practical result: an L-shaped part with 50 and 50 legs in 2 mm sheet does not unfold to 100 — it unfolds to about 97. The difference comes from the bend itself.
This is why you should supply the flat pattern yourself. Leave the shop to compute it and they will use their machine's K-factor, which may not be the one you assumed.
Hole-to-bend distance
A hole too close to the bend line gets stretched into an oval during forming.
Rule: edge of hole to start of bend ≥ 2.5 × thickness + bend radius.
For 2 mm sheet with a 2 mm radius: at least 7 mm from hole edge to bend line.
If you must place a hole closer, you have two options: drill after bending (more expensive), or add a small relief cut along the bend.
Minimum flange length
A very short flange cannot be gripped in the press brake and will not fold.
Rule: minimum flange ≈ 4 × thickness + bend radius.
For 2 mm sheet, a flange shorter than about 10 mm is effectively unbendable.
Bend sequence
A part with four bends may collide with the machine on the third. This has to be considered at design time.
Simple rule: work from inner bends outward, and if the part closes into a box, make sure the tool still has room for the last fold.
If in doubt, check the drawing with the shop. A five-minute call is cheaper than a scrapped part.
Cutting: which process
| Process | Typical thickness | Accuracy | Edge quality |
|---|---|---|---|
| Laser | to 20 mm steel | ±0.1 mm | Excellent, almost burr-free |
| Plasma | to 50 mm | ±0.5 mm | Moderate, tapered edge |
| Waterjet | to 150 mm | ±0.2 mm | Good, no heat-affected zone |
| Punching | to 6 mm | ±0.2 mm | Good, high volume only |
Kerf (cut width) on a laser is about 0.2 mm. Irrelevant for ordinary parts, but it must be accounted for if two pieces have to nest exactly.
Choosing the sheet
- Mild steel (ST12/ST37) — cheapest, needs paint or galvanising
- Galvanised — rust resistant, but welding burns the coating and produces toxic fumes
- Stainless 304 — corrosion resistant, dearer, harder to bend (more springback)
- Aluminium — light, but needs a larger bend radius and scratches easily
Five expensive mistakes
1. Not supplying the flat pattern. The shop computes its own and the finished dimensions differ from your model.
2. Zero bend radius in the model. The unfold is wrong.
3. Holes too close to a bend. They come out oval.
4. Forgetting springback. Stainless and aluminium spring back after forming; the shop compensates, but it needs to know.
5. Sharp internal corners. A laser cannot cut a perfectly sharp internal corner; a small radius always remains. Model it in.
If you have a part currently machined from solid, it is worth checking once whether it could be redesigned as sheet metal. Often the answer is yes, and the saving is substantial.