RODEx / Articles / Sheet metal flat pattern calculator

Sheet metal flat pattern calculator

18 October 2026 · RODEx

Short answer: flat pattern length = sum of outside flange dimensions − number of bends × bend deduction. Bend deduction BD = 2·(r + s)·tg(α/2) − BA, where the bend allowance is BA = π·α/180·(r + K·s). Everything comes down to the factor K — and references give it differently, so the calculator below shows the spread right away.

Flat pattern calculator

Sheet thickness s, mm Inner bend radius r, mm Bend angle, ° Outside flange dimensions, mm (comma-separated, decimals with a dot)

K factor reference table DIN 6935 formula own (shop table)

Blank length (flat pattern)—

K—

Bend allowance per bend, BA—

Bend deduction per bend, BD—

Bends—

What is the K factor

When bending, the outer side of the sheet stretches and the inner side compresses; between them is the neutral layer, whose length does not change. K — where this layer lies, as a fraction of thickness from the inner side: 0 is at the inner surface, 0.5 is in the middle. The tighter the bend (smaller r/s), the closer the layer to the inner side and the smaller K. The flat pattern length is the length of the neutral layer.

K versus r/s: sources disagree

r/s	Reference table x₀ steel 10–20, 90° bend	Table k by R and S, mm	DIN 6935 formula K = (0.65 + 0.5·lg(r/s))/2
0.5	0.38	—	0.25
1	0.42	0.35	0.33
2	0.45	0.375	0.40
3	0.47	0.40	0.44
5	0.48	0.43	0.50

For a 2 mm sheet with a 4 mm radius (r/s = 2), three sources give K from 0.375 to 0.45. On one 90° bend that is a bend allowance difference of about 0.24 mm, on a part with four bends — about a millimetre. For laser cutting and press braking that matters.

Why: K depends not only on r/s but also on the bending method (air bending or bottoming), tooling, material grade and rolling direction. References average different conditions.

How to get your own K in 10 minutes

Cut a strip of known length L from the same sheet.
Bend it to 90° on the same machine and tooling that will run the batch.
Measure the outside flange dimensions A and B.
Bend deduction: BD = A + B − L. Bend allowance: BA = 2·(r + s) − BD. K factor: K = (BA·2/π − r) / s.

Enter this K in the calculator (“own”) and your flat patterns will match your shop. Many shops already keep such a bend table: ask for it — we calculate flat patterns from it.

Before you cut the blank

K comes from the shop’s bend table or a test bend, not from the internet
Radius r is the inside radius, the one the shop’s tooling produces
Flange dimensions are outside dimensions (to the virtual sharp)
The flat pattern was “folded back” in 3D and compared with the part

Tick what you have already checked

Don’t want to calculate by hand?

We’ll make the DXF flat pattern from your drawing

Cutting contour, bend lines, bend table (from your shop’s table if you send it) and a 3D model — usually in 10–30 minutes. We fold every flat pattern back and compare it with the part. Price ($8 in the pilot) — before you pay.

Upload a drawing

Questions and answers

Which K to use if the shop has no table?

For ordinary steel at r/s from 1 to 3, references give 0.35–0.47. For the first part take the reference value and make a test bend: K is calculated from it in a minute (formula in the article).

Why do online calculators give different flat pattern lengths?

They take K from different tables or formulas. For a 2 mm sheet and a 4 mm radius that is 0.375 to 0.45 — a difference of about 0.24 mm per bend.

How does bend allowance differ from bend deduction?

Bend allowance BA is the length of the neutral layer in the bend zone: it is added to the straight sections. Bend deduction BD is how much to subtract from the sum of the outside flange dimensions. Two ways to calculate the same thing.

Does the calculator work for cones and shells?

No: this is for straight-line sheet bends. Cone and shell flat patterns use other formulas.