Sheet Metal Bend & K-Factor Calculator — Flat Pattern
Industrial-grade bending calculator: K-factor from R/T ratio, bend allowance, outside setback, bend deduction, flat-pattern length, minimum radius and flange checks, V-die selection, press-brake tonnage and full audit trail.
Decision:Run the stated engineering model, review its assumptions and warnings, then make the release decision against the governing standard and verified source data.
SectorCalc SC-030 computes the flat pattern of a bent sheet-metal part: bend allowance from the K-factor neutral-axis model, outside setback, bend deduction, and flat length from apex-measured legs. K is estimated from the R/T ratio per DIN 6935 practice or entered from your own bend trials — the only fully reliable source. Tooling checks cover minimum inside radius, minimum flange, V-die opening and press-brake tonnage per metre. Flat patterns from any K-factor are first-article estimates: cut one blank, measure, correct K, then release.
The neutral axis and K-factor
K = tn / T (neutral axis offset from inside face)
K ≈ 0.33 + 0.17 · (R/T) / (1 + R/T) (air-bend practice)
The inside of the bend compresses, the outside stretches; only the neutral fibre keeps its length. At tight radii (R < T) the neutral axis shifts inward toward K ≈ 0.33–0.40; at large radii it approaches the mid-plane K = 0.5. Material, grain direction and die opening all move it — auto-K is a starting value, not a measurement.
Bend allowance, setback, deduction
BA [mm] = θ[rad] · (R + K·T)
OSSB = tan(θ/2) · (R + T)
BD = 2·OSSB − BA
Bend allowance is the arc length of the neutral fibre; setback is what the apex geometry adds; deduction is what you subtract from the sum of apex-measured legs. All three are shown because different CAD and shop conventions use different ones — mixing them up is the classic source of 1–2 mm flange errors.
Flat-pattern length
Lflat = L1 + L2 − BD (legs measured to the apex)
For multiple bends, repeat per bend and subtract each deduction. Legs must use one convention — this engine takes outside-face-to-apex, the press-brake standard. CAD mold-line dimensions need the mold-line variant: L = (L1−OSSB) + (L2−OSSB) + BA, identical result.
Minimum radius and minimum flange
Cracking on the outside fibre governs the tightest radius: soft aluminium ≈ 0.5·T, mild steel ≈ 1.0·T, stainless ≈ 2·T, hard aluminium (T6) ≈ 3·T — doubled across the rolling grain. The shortest flange that seats on a V-die is ≈ 0.7·V + R; below it the sheet falls into the die and the angle is lost.
V-die selection and tonnage
F [t/m] = 1.42 · Rm[kgf/mm²] · T² / V
Air-bending tonnage scales with the square of thickness and inversely with die opening — 3 mm in V16 needs four times the force of 1.5 mm in V16, not twice. Machine capacity must also cover tooling load limits (t/m of the punch), which are frequently lower than the press rating.
Frequently asked questions
My flat is 1.5 mm short — which input is wrong?
Nine times out of ten, K. Cut one blank, bend, measure the flanges, and solve K backwards from the error. Material batch-to-batch yield variation moves K by 0.02–0.05, worth ~0.5 mm on a 90° bend in 2 mm steel.
Why does the same part bend differently across grain?
Rolling elongates grains; bending across the grain is more ductile. Along-grain bends need larger radii (double for stainless and hard aluminium) and show more springback. Nest grain direction into the cutting plan.
How much springback should I expect?
Air bending mild steel: 0.5–2°. Stainless and HSLA: 2–5°, sometimes more at large R/T. This engine flags high springback risk; compensation is done by over-bending in the press program, not in the flat pattern.
Bottoming vs air bending?
Bottoming (coining the radius) kills springback and sets K ≈ 0.33–0.40 but needs 3–5× the tonnage and dedicated dies per thickness/angle. Air bending with one V-die per thickness range is the modern default; the tonnage formula above is air bending.
