K-Factor and Bend Allowance for Sheet Metal Bending

K factors by material and thickness for air bending, bottoming and coining per DIN 6935, with bend allowance and deduction worked examples for 90-degree bends.

K factors by material, thickness and bend method (calculated DIN 6935 + published ranges)

What K-factor should I use for 2 mm mild steel in air bending?

At R/t = 1 (R = 2 mm), DIN 6935 gives K = 0.325 (0.33 rounded); the common CAD default 0.44 adds about 0.36 mm per 90° bend. Full flat-pattern check below.

Why do CAD programs default to a K-factor of 0.44?

It is a historical mild-steel default (0.44–0.45), not a universal value: for 5052 aluminium the same default is about 0.33–0.40, and for 304 stainless 0.40–0.45. DIN 6935 at R/t = 1 gives 0.325 — do not average the two calibers; test-bend and back-solve instead.

How does K-factor change with inside radius?

It rises toward 0.50 as R/t reaches 5: DIN 6935 gives K 0.25 at R/t = 0.5, 0.33 at 1.0, 0.40 at 2.0 and 0.45 at 3.0. Interpolate between rows with k = 0.65 + 0.5·log10(R/t), never linearly.

What is the difference between air bending, bottoming and coining in K-factor?

Published starting values are 0.33–0.45 for air bending, 0.42–0.48 for bottoming and 0.38–0.47 for coining; never use an air-bend K for bottoming. These are starting values, not standard values.

How do I calculate bend allowance?

BA = (π/180) × A × (R + K × t); for 2 mm mild steel, R 2 mm, K 0.325, 90° gives 4.163 mm. A is the bend angle — the angle the sheet travels: a 60° included angle means A = 120°.

How do I calculate bend deduction?

BD = 2 × OSSB − BA; the same 90° bend has OSSB 4.000 mm and BD 3.837 mm, so 50 + 30 mm outside flanges develop to 76.16 mm. The non-90 example cross-checks the same ledger at A = 120°.

What V-die opening should I use for 2 mm mild steel?

Start at V16 (8 × t); it gives an inside radius near 2.6 mm, a minimum flange over 11 mm and about 12 t/m in 60,000 psi mild steel. Stainless wants V = 10–12×t and a 20–22% radius factor.

What K-factor should I use for 304 stainless?

Use 0.40–0.45: DIN 6935 gives 0.41 at R/t = 2.1, while the published hard-material starting value is 0.45; 316 runs higher, up to 0.45–0.50 in shop data — take the upper bound and test-bend.

What K-factor should I use for 5052 aluminium?

Use 0.34–0.40; 5052-H32 at R/t ≈ 1.2 sits near 0.33–0.35, while a generic soft-aluminium table gives 0.40 for R = t–3t. Keep 6061-T6 on its own row — do not mix it with 5052.

Can I use one K-factor for all thicknesses?

Only if V/t and R/t stay constant; a 0.5 mm sheet on a practical V6 die runs R/t ≈ 1.9 and K ≈ 0.40, while 2 mm on V16 runs R/t ≈ 1.3 and K ≈ 0.35. Thickness moves K through the die, not through the formula.

How do I measure the real K-factor for my press brake?

Bend a 200 mm strip at 90°, measure both outside flanges, get BD = 200 − (A + B), then back-solve K from K = [2(R + t)tan(A/2) − BD] / [(π/180)At] − R/t. Write the measured K back into the CAD library and stop reusing 0.44 for that material/tooling pair.

Where is the neutral axis in a bend?

At y = K × t from the inside surface: 2 mm mild steel with K 0.35 puts it 0.70 mm from the inside, so the neutral radius is R + 0.70 mm.

Why does coining sometimes show a lower K than bottoming?

The published table gives coining 0.44–0.47 versus bottoming 0.46–0.48 in the R = t–3t range, which is the opposite of the usual expectation that coining pushes K toward 0.50 — treat it as an unresolved conflict and verify with a test bend.

How to Use These Numbers

• Table rows are calculated values plus published starting ranges — never present them as measured K factors; the DIN column is a formula value and the published columns are CAD/shop starting values that differ from it by 0.03–0.09.
• 0.44 is a historical CAD default, not the K-factor of mild steel: DIN 6935 gives 0.325 at R/t = 1. If a CAD flat pattern will not fit the bent part, check which caliber the software used before touching the tooling.
• Both worked examples use the K values consistent with Table 1 (0.325 at R/t = 1, 0.40 at R/t = 2) — do not swap in 0.44 to make the arithmetic prettier.
• DIN 6935 targets ductile, medium-strength steels; the aluminium, copper and brass rows borrow only its geometry, with the published ranges covering the hardening difference. 6061-T6 is marked * because no DIN-caliber table exists for it — test-bend is mandatory.
• Titanium Grade 2, HSLA steels and Inconel have no citable K tables — back-solve K from a test bend instead of guessing; thicknesses above 6 mm, hems, curling and joggles are outside this table's scope.
• Springback is a separate compensation: K locates the neutral axis but does not give the springback angle; compensate per material and die, not from this table.
• The DIN 6935 original was not purchased; the formula and k table are verified against two independent public sources (a technical digest and a software implementation that agree value by value) — re-verify against the purchased standard before production-critical use.

Frequently Asked Questions

Standards & Sources

• S1 — Rainer Schlangen, Biegetechnik — Biegeverkürzung (2010): DIN 6935 digest — k = 0.65 + 0.5·log10(r/s), k table 0.05–5.0, K = k/2, neutral layer NT = (s/2)·k
• S2 — Protolabs Network (ex-Hubs), Sheet metal fabrication design guide — generic K-factors for air/bottoming/coining, soft–medium–hard, default 0.4468
• S3 — ADH Machine Tool, Press Brake V Die Opening Chart — 8×t start, R_i ≈ 16% V, stainless 10–12×t at 20–22%; rows for 1.0–6.0 mm verified against the published chart
• S4 — Lapas, K-Factor and Bend Allowance — material-at-R=t shop calibers: 5052 0.33, 6061-T6 0.40, A36 0.44, 304 0.46, 316 0.50; R/t > 3 → K ≈ 0.50
• S5 — MechCodex, Sheet Metal K-Factors by Material and Bend Method — cross-check of S2
• S6 — smlibpy, Sheet metal: what the functions share — independent DIN 6935 formula implementation, K = k/2, default 0.44
• S7 — DIN 6935 Kaltbiegen von Flacherzeugnissen aus Stahl (paid standard, not purchased; cited only as the upstream of S1/S6)

Related Pages

• /wiki/sheet-metal/bend-radius-and-bend-allowance/ — Long-form guide: inside radius selection and bend allowance practice
• /wiki/sheet-metal/tolerance-and-surface/ — Sheet metal tolerances and finish expectations formed parts are held to
• /wiki/sheet-metal/design-for-sheet-metal/ — DFM rules for bends, flanges and reliefs that set R/t in the first place

Download This Table

• CSV
• JSON
• Markdown