Engineering · Design for Manufacturing · 3 of 8
DFM for Sheet Metal
Will the flat blank fold into the part you drew, without cracks, oval holes or a tooling change?
Sheet metal parts are cheap when they follow the shop’s bending rules and expensive when they do not. Most trouble comes from five things: too small a bend radius, features too close to a bend, no relief at corners, odd flange sizes and springback. This page gives the rules in thickness multiples and four calculators: bend allowance and flat length, feature-to-bend distance, relief size and overbend.
1Material selection
| Material | Common grades | Thickness (mm) | Key points | Typical use |
|---|---|---|---|---|
| Mild steel (CRCA) | IS 513 / SPCC | 0.5 to 6.0 | Low cost, good forming, easy to weld | Enclosures, brackets, frames |
| Stainless steel | SS304, SS316 | 0.5 to 6.0 | Corrosion resistant, springs back more | Food, pharma, outdoor equipment |
| Aluminium | 5052, 6061 | 0.5 to 4.0 | Light, corrosion resistant, bigger bend radius | Panels, covers, lightweight structures |
| Galvanised steel | GI (Z60, Z120) | 0.5 to 3.0 | Corrosion resistant, moderate forming | Electrical cabinets, HVAC |
| Pre-painted steel | PPGI | 0.5 to 2.0 | Good appearance, protect the coating at the bend | Consumer products, enclosures |
Choose from the sheet sizes and grades your supplier stocks. Special thickness and grades add lead time.
2Bend allowance and flat length
The flat blank is shorter than the sum of the outside legs, because the metal in the bend stretches. Enter the bend and get the flat length.
Bend calculator
OSSB = tan(A/2) × (R + T)
BD = 2 × OSSB − BA
flat length = leg 1 + leg 2 − BD
Legs are measured to the outside of the bend, as on a normal drawing. A is the angle the sheet is turned through (90 for a right angle). K is usually 0.3 to 0.5 and depends on material and tooling; ask the shop for its value.
| Material | Recommended minimum inside radius R |
|---|---|
| Mild steel (CRCA) | 0.5 to 1.0 × T |
| Stainless steel | 1.0 to 1.5 × T |
| Aluminium | 1.0 to 2.0 × T |
| Galvanised steel | 0.8 to 1.5 × T |
| Pre-painted steel | 1.0 to 1.5 × T |
A radius below the minimum can crack the bend, spoil the finish or cause springback trouble. Use one standard radius for the whole part where you can.
3Hole to bend distance
Feature-to-bend checker
| Feature | Minimum distance |
|---|---|
| Round hole | ≥ 2.0 × T |
| Slotted hole (width) | ≥ 2.5 × T |
| Square hole | ≥ 2.0 × T |
| Notch or cut-out | ≥ 2.5 × T |
Closer than this and the hole stretches into an oval. Measure from the hole edge to where the bend starts, not to the bend line.
4Bend relief
Relief size
| Thickness T | Relief width W | Relief depth D |
|---|---|---|
| up to 1.0 mm | 1.0 × T | 1.0 × T |
| 1.0 to 2.0 mm | 1.5 × T | 1.5 × T |
| over 2.0 mm | 2.0 × T | 2.0 × T |
The rectangular relief is the common choice. A tear-drop relief (diameter at least T, slot width about 1.5 T) is stronger against fatigue cracks because it has no sharp corner. The relief gives the material room to deform without tearing at the corner.
5Flanges, hems and joggles
Minimum feature sizes
Values are typical for press-brake work. A flange shorter than about 4 T may not sit in the die and can twist or slip. Check your shop’s tooling.
6Springback
Overbend estimate
Springback ranges are typical. Bigger inside radius and thinner, stronger material give more springback. The shop compensates by overbending in the tooling, so do not specify a tolerance tighter than the process can hold.
7Common design mistakes
Bend radius too small
Causes cracks and a poor finish.
Hole too close to bend
Distortion and oval holes.
No bend relief
Material tears at the bend corner.
Many bends in one edge
Difficult to make and costs more.
Unnecessary tight tolerances
Cost goes up with no benefit.
Odd radii and flange widths
Extra tooling and set-up changes.
8Good and poor design
Good design
- Standard bend radius and standard flange widths.
- Adequate hole-to-bend distance.
- Simple, symmetric geometry.
- Recessed fasteners and standard bends on enclosures.
Poor design
- Tight radius, no relief, hole near the bend.
- Complex bends and cut-outs that are hard to hold.
- Unnecessary features that add cost.
9Try it: DFM checklist for sheet metal
Sheet metal DFM scorecard
Remember
- Inside radius at least the material’s minimum, and one standard radius where possible.
- Holes at least 2 T from a bend; slots and notches at least 2.5 T.
- Add bend relief; keep flanges at least 4 T.
- Flat length = legs minus bend deduction; confirm K-factor with the shop.
- Boothroyd, Dewhurst and Knight, Product Design for Manufacture and Assembly (CRC Press), for the DFM and DFA method.
- Machinery’s Handbook (Industrial Press), for machining, sheet metal and welding practice.
- Bend allowance method: standard K-factor formulas as used in sheet metal handbooks and CAD systems.
- IS 513 (cold-rolled steel sheet) and the usual 304/316, 5052/6061 grades.
Minimum radii, K-factors and springback values are typical. They depend on grade, temper, grain direction and tooling. Ask the fabricator for its press-brake data before release.