Sheet metal flat patterns: bend allowance and K-factor
A bent sheet-metal part is cut flat first and bent afterwards. How long must the flat blank be? Not the sum of the outside lengths: when the sheet bends, the outside surface stretches and the inside is compressed, and only one line keeps its length — the neutral axis. Calculating a flat pattern means finding the length along that axis.
Terms
| Value | Meaning |
|---|---|
| T | Sheet thickness |
| R | Inside bend radius |
| A | Bend angle (how far the sheet is bent; a right-angle bend = 90°) |
| K (K-factor) | Position of the neutral axis from the inside surface, as a fraction of the thickness (0 = inside, 0.5 = middle) |
| BA (bend allowance) | Length of the bend along the neutral axis |
| BD (bend deduction) | What to subtract from the sum of the outside lengths |
Formulas
BA = π × A / 180 × (R + K × T)
BD = 2 × (R + T) × tan(A / 2) − BA
Flat length = (sum of all outside lengths) − BD × (number of bends), or = (sum of the straight parts) + BA × (number of bends).
Example: a 90° bracket in 2 mm sheet
An L-shaped part, 50 × 30 mm outside, thickness T = 2 mm, inside radius R = 2 mm, K = 0.4.
- BA = π × 90 / 180 × (2 + 0.4 × 2) = 1.5708 × 2.8 ≈ 4.40 mm
- Straight part of each leg = outside length − (R + T): long leg 50 − 4 = 46, short leg 30 − 4 = 26
- Flat length = 46 + 26 + 4.40 = 76.40 mm
- Check with BD: 2 × (2 + 2) × tan 45° − 4.40 = 8 − 4.40 = 3.60 → 50 + 30 − 3.60 = 76.40 mm, the same
Simply adding the outside lengths gives 80 mm — 3.6 mm too long, and the bent part comes out oversize.
Which K-factor to use
| Bending condition | Approximate K |
|---|---|
| Bend radius smaller than thickness (R < T), bottoming | 0.30–0.35 |
| Air bending, R about 1–3 × T, general steel sheet | 0.40–0.45 |
| Very large radius (R > 3T) | 0.45–0.50 |
These are starting values only; the real K depends on the material, the tooling and the press brake. The most accurate way is to bend a test piece, measure it and work K out backwards — or ask the bending shop for its BD table. Most shops have one for their own machines.
Drawing the flat pattern in DXCAD2D Online
- Draw the flat blank at the calculated length — for example
REC, click the first corner at 0,0 and type76.4,40for a 40 mm wide blank. - Draw the bend line at 46 + BA/2 = 48.2 mm from the edge on its own layer, with a centre or dashed line type (the shop uses it as the centre of the bend).
- Draw holes and slots in their positions on the flat blank. Keep holes near a bend at least about 2T + R from the bend line, or they distort when bent.
- Export the DXF for cutting: hide the bend-line and text layers first if the shop wants only cutting lines, or keep them on separate layers and tell the shop which layer is the bend line.
- Always send a PDF of the bent part with outside sizes, bend angles, bend direction (up/down) and radius together with the flat DXF.
Try it right now — a free 2D CAD in your browser. Nothing to install, no sign-up.
Open DXCAD2D OnlineThings to watch
- Minimum bend radius. Hard or thick sheet cracks on the outside if the radius is too small — especially hard aluminium grades. Ask the shop which radii its tooling makes.
- Minimum flange length. A flange that is too short cannot be bent because it does not span the die. As a rough guide keep it at least about 3–4 times the thickness (it depends on the die opening).
- Bend relief. Where a bend line runs into an edge, cut a small relief slot at the end of the bend, at least as wide as the thickness, so the sheet does not tear.
- Grain direction. Rolled sheet has a direction; bending across the rolling direction cracks less than bending along it.
- Tolerances. Bent parts vary more than machined ones. Do not put fine tolerances on sizes that cross a bend — see ISO 2768 tolerances.
More on preparing cutting files in preparing drawings for laser cutting.