About Bend Allowance Calculator — K-Factor, Bend Deduction & Flat Pattern
The bend allowance calculator turns a bent part into its flat-pattern length. When sheet metal bends, the material along the inside compresses and the outside stretches; somewhere between lies the neutral axis that keeps its length. The K-factor locates that axis as a fraction of the thickness (t = K·T from the inside face), so the arc the flat pattern must supply is BA = θ·(π/180)·(R + K·T) — the bend allowance.
From the same geometry the tool derives the outside setback OSSB = (R+T)·tan(θ/2) — the distance from the outside mold-line intersection back to each bend tangent — the bend deduction BD = 2·OSSB − BA, and the flat length: add the two flange outside dimensions and subtract BD. The default K of 0.44 is the industry baseline for air-bent low-carbon steel over a die opening near 8× thickness; air bending generally lands between 0.40 and 0.45.
How It Works
- Enter the material thickness and the inside bend radius. For air bending the inside radius is set by the die opening, not the punch tip — a common estimate is around 1/6 of the V-die opening for mild steel; use your shop's measured value when you have one.
- Set the K-factor. 0.44 suits air-bent mild steel; harder bending (smaller radius relative to thickness, bottoming) pulls the neutral axis inward toward 0.40 or below, gentler forming with large radii pushes it toward 0.50 (it can never exceed 0.50 — the axis cannot sit past mid-thickness).
- Enter the bend angle as the complementary (outside) angle — 90° for a square corner — and the two flange lengths measured to the outside mold line, the way a part is dimensioned on a print.
- Read the results: bend allowance (the neutral-axis arc), outside setback, bend deduction, and the flat-pattern length A + B − BD. The tool checks that each flange at least covers the setback — a shorter flange cannot form the bend.
- For angles past 90° the tan(θ/2) setback convention no longer applies (it diverges toward 180°), so the tool reports the bend allowance only — still exactly the neutral-axis arc — and leaves the deduction to your CAD system's obtuse-bend convention.
Worked Example
A bracket in 2 mm mild steel is bent 90° over a 3 mm inside radius with two 50 mm flanges (outside dimensions). Neutral radius: 3 + 0.44 × 2 = 3.88 mm, so the bend allowance is (π/2) × 3.88 = 6.095 mm of arc. Outside setback: (3 + 2) × tan(45°) = 5 mm; bend deduction: 2 × 5 − 6.095 = 3.905 mm. Cut the blank at 50 + 50 − 3.905 = 96.095 mm — about 96.1 mm — and the finished legs land on 50 mm each. Cutting at the naive 100 mm would leave both flanges nearly 2 mm long, because the material only "uses up" 6.1 mm of length around the corner while the outside dimensions overlap by 10 mm.
Formulas
- Bend allowance (neutral-axis arc)
BA = θ × (π/180) × (R + K·T)- Outside setback (θ ≤ 90°)
OSSB = (R + T) × tan(θ/2)- Bend deduction and flat pattern
BD = 2 × OSSB − BA; flat = A + B − BD
Standards & References
- K-factor neutral-axis flat-pattern method as documented in press-brake references (The Fabricator, "K-factors, Y-factors, and press brake bending precision") and implemented by CAD sheet-metal engines
- Default K = 0.44: industry baseline for air-bent low-carbon steel with a V-die opening near 8× material thickness; air bending typically produces K ≈ 0.40–0.45 (The Fabricator)
- K physically bounded below 0.50 (the neutral axis can shift only inward from mid-thickness); published charts rarely run below ≈0.30 even for severe coining
Frequently Asked Questions
What is a K-factor in sheet metal bending?
The K-factor is where the neutral axis — the fiber that neither stretches nor compresses — sits through the bend, expressed as a fraction of material thickness measured from the inside face. K = 0.44 means the neutral axis lies at 44% of the thickness. It exists because bending shifts the neutral axis inward from the geometric middle (0.50); how far depends on material, radius-to-thickness ratio, and bending method.
What K-factor should I use for steel?
Start at 0.44 for air-bent low-carbon steel — the industry-standard baseline that most CAD systems ship as their default, derived from air bending over a V-die opening near 8× thickness. Tighter radii and bottoming drive K down toward 0.40; large-radius gentle bends drift up toward 0.50. For production accuracy, bend a test coupon, measure the flat that produced the right part, and back-solve K — a measured K always beats a chart.
What is the difference between bend allowance and bend deduction?
Bend allowance (BA) is the arc length of material actually in the bend — what you add when working from tangent-to-tangent flat dimensions. Bend deduction (BD) is what you subtract when the part is dimensioned to the outside mold lines, the common print style: flat = A + B − BD. They encode the same physics, related through the setback: BD = 2·OSSB − BA. This tool reports both so you can work either way.
How do I calculate the flat pattern for a 90 degree bend?
Add the two outside flange dimensions and subtract the bend deduction. For 2 mm steel on a 3 mm inside radius: BA = (π/2)(3 + 0.44×2) = 6.095 mm, OSSB = (3+2)·tan 45° = 5 mm, BD = 2×5 − 6.095 = 3.905 mm, so two 50 mm flanges cut flat at 96.095 mm. Multi-bend parts subtract one BD per bend.
Why does the calculator stop reporting setback above 90 degrees?
The outside setback formula (R+T)·tan(θ/2) is the distance from the outside corner intersection to the bend tangent, and past 90° that tangent intersection geometry changes while tan(θ/2) races toward infinity at 180°. CAD systems switch conventions for obtuse bends. The bend allowance itself — the neutral-axis arc θ(π/180)(R+K·T) — stays exact at any angle, so the tool keeps reporting it and leaves obtuse deductions to your CAD convention.
Does the inside radius equal my punch-tip radius?
Not in air bending — the sheet floats across the V-die and takes a natural radius set mostly by the die opening (roughly 1/6 of the V width for mild steel), as long as that is larger than the punch tip. Only bottoming and coining force the sheet onto the punch radius. Measure a test bend or use your tooling chart; the radius feeds both BA and OSSB, so an assumed radius that is off by a millimetre moves the flat pattern visibly.