IDB-SMD-038
Sheet metal · bends · K-factor · DFM
Sheet-metal design guide
Designing bent sheet-metal parts — bend allowance and the K-factor, minimum bend radii and reliefs, hole and edge rules, and the DFM that keeps parts cheap and accurate.
Abstract
Sheet-metal parts are cut flat (laser/punch) and folded on a press brake, so the design problem is two-fold: lay out features that survive bending, and compute a flat pattern that folds to the right finished size. The bend allowance and K-factor handle the second; min-radius, relief and edge rules handle the first.
Section 1 is DFM fundamentals. Section 2 is bend allowance and the K-factor. Section 3 is minimum bend radius and reliefs. Section 4 is holes, slots and edge distances. Section 5 is forming features and hardware. Section 6 is cost and a checklist. A companion Excel bend calculator computes BA / BD / flat length live.
1.DFM fundamentals
Sheet metal is one constant thickness, cut flat then formed — so design with that grain:
- One material thickness per part; pick a standard gauge.
- Bends are cheap, cuts are cheap; complexity in setups is notminimise the number of bends and unique bend angles.
- Uniform everythingconsistent bend radius across the part lets one tool do all bends.
- Typical process: laser/punch the flat blank → press-brake the bends → hardware (PEM) → finish.
2.Bend allowance and the K-factor
When sheet bends, the outside stretches and the inside compresses; the neutral axis (length unchanged) lies at K·t from the inside surface. The flat pattern length follows from it:
- Bend allowance
BA = θ_rad · (R + K·t)(θ = bend angle, R = inside radius) - Outside setback
OSSB = (R + t)·tan(θ/2) - Bend deduction
BD = 2·OSSB − BA - Flat length (single bend, outside legs A and B)
= A + B − BD
K depends on radius/thickness ratio and material; use ≈0.40 as a default, then refine from test bends or the brake's data:
| Condition | Typical K |
|---|---|
| Soft material / small R (R < t) | ~0.33 |
| General (R ≈ t) | ~0.40 |
| Hard material / large R (R > 2t) | ~0.45 |
The companion Excel calculator computes BA, BD and flat length from t, θ, R and K live.
3.Minimum bend radius and reliefs
- Minimum inside radius rises with thickness and hardness. Bending tighter cracks the outside fibre, especially across the grain:
| Material | Min inside radius |
|---|---|
| Soft aluminium (5052-O) | 0.5–1 × t |
| Mild steel | ~1 × t |
| Stainless / half-hard | 1–2 × t |
| Hard tempers (6061-T6) | 2–3 × t |
- Bend relief: add a relief notch (≥ t wide, ≥ t deep) where a bend ends at an edge, or the corner tears.
- Bend orientation: bend across the rolling grain where possiblebends parallel to the grain crack sooner.
4.Holes, slots and edge distances
Punched/laser features need clearance or they distort during bending:
| Feature | Rule of thumb |
|---|---|
| Min hole / slot diameter | ≥ material thickness t |
| Hole / slot to edge | ≥ 2 × t |
| Hole / slot to bend | ≥ 2.5 × t + R (else it deforms) |
| Min flange length (leg) | ≥ 4 × t + R (to grip the brake) |
| Notch / tab width | ≥ 2 × t |
5.Forming features and hardware
- Hems (folded edges) stiffen and remove sharp edges; allow ~ flat-hem clearance.
- Countersinks in thin sheet are shallowlimit to ~0.6 × t depth or use extruded holes.
- Louvers, ribs, embosses stiffen a panel cheaply versus adding thickness.
- Press-in hardware (PEM nuts/studs) add threads without weldingrespect the vendor's min sheet thickness and edge distance.
- Tolerances: bends carry ±0.1–0.5 mm and angular ±0.5–1° typically; don't stack tight tolerances across multiple bends (see Tolerance stack-up).
6.Cost and checklist
- Fewer bends, one radius, standard gaugethe three biggest cost levers.
- Avoid tight tolerances across bendseach bend adds variation.
- Nest-friendly flatsimple outline, minimal scrap.
- Checklist: standard thickness → consistent bend radius ≥ min for the material → features ≥ rules above from edges/bends → bend reliefs at edges → compute the flat pattern (BA/BD via the calculator) → realistic bend tolerances → hardware edge distances.