Skip to main content

Free tool

Bend allowance, bend deduction & K-factor calculator

Bend allowance and bend deduction are the two numbers that convert a formed part's flange lengths into a flat pattern, and back again. Enter material thickness, inside bend radius, bend angle, and K-factor below for live results, or scroll past the calculator for the formulas, a worked example, and a reference table.

Calculator

Presets are typical starting values; verify with a test bend.

Bend allowance

0.1338in

Setback

0.1200in

Bend deduction

0.1062in

Flat length — two-flange part

Flat pattern length

1.8938in

Results are theoretical. Production values depend on your actual tooling, bend method (air vs. bottom vs. coin), and material lot — we verify every locked program with a first-article bend before running production.

The formulas

These are the standard bend-allowance and K-factor formulas used across sheet-metal design and fabrication references — the same neutral-axis geometry taught in manufacturing engineering courses and formalized in sheet-metal bending standards. Every length below (T, R, F1, F2) must be entered in the same unit; the calculator above handles that conversion for you.

Bend allowanceBA = (π / 180) × A × (R + K × T)

Outside setbackOSSB = tan(A / 2) × (R + T)

Bend deductionBD = 2 × OSSB − BA

Flat length, two flangesFlat = F1 + F2 − BD

Where:

  • T — material thickness
  • R — inside bend radius
  • A — bend angle, in degrees
  • K — K-factor, the neutral-axis ratio t ⁄ T
  • F1, F2 — flange lengths, measured to the outside mold line (where the flange faces would meet if extended to a sharp virtual corner)

Worked example

T = 0.060 in, R = 0.060 in, A = 90°, K = 0.42 (mid-range mild steel/CRS air-bend value) — the same numbers the calculator above loads by default.

  • BA = (π / 180) × 90 × (0.060 + 0.42 × 0.060) = (π / 2) × 0.0852 = 0.1338 in
  • OSSB = tan(45°) × (0.060 + 0.060) = 1 × 0.120 = 0.1200 in
  • BD = 2 × 0.1200 − 0.1338 = 0.1062 in
  • Flat length at F1 = F2 = 1.000 in: 1.000 + 1.000 − 0.1062 = 1.8938 in

What is K-factor?

K-factor is the ratio that locates a bent sheet's neutral axis — the internal layer that neither stretches nor compresses through the bend — relative to the material's inside surface. Expressed as K = t / T, where t is the distance from the inside face to the neutral axis and T is material thickness, K-factor is what turns bend geometry (radius, angle, thickness) into an accurate flat-pattern length.

K is not a fixed material constant. It shifts with bend method (air bending pushes the neutral axis further toward the inside face than bottom bending or coining), the ratio of inside radius to thickness, material temper and grain direction, and tooling geometry. That's why published K-factor tables give ranges, not single numbers — air-bending mild steel commonly sits around 0.40–0.45, soft aluminum lower around 0.33–0.38, and stainless higher around 0.45–0.50, because stainless work-hardens and springs back more through the bend.

For a first pass — quoting, DFM review, comparing part designs — the typical range for your material family is a reasonable starting point. For a production part where flat-pattern accuracy actually matters, the only reliable number is the one measured from an actual test bend on your material, thickness, and tooling. Treat every K-factor on this page as a starting value, not a guarantee.

Common mistakes

  • Using one "default" K-factor for every material and process. CAD software defaults (often around 0.44) are calibrated to one representative case, not necessarily your material and tooling.
  • Confusing bend allowance with bend deduction. BA is the material consumed inside the bend, measured along the neutral axis; BD is what you subtract from flange lengths measured to the outside mold line. Mixing them up throws off the flat pattern by roughly the difference between the two.
  • Measuring flange lengths to the wrong reference. The flat-length formula above expects flange lengths measured to the outside mold line — where the two flange faces would meet if extended to a sharp virtual corner — not to the tangent point of the bend radius.
  • Assuming the programmed radius is the actual radius. Air bending doesn't fully seat the material into the die, so the true inside radius depends on punch geometry and overbend — not just the die's nominal radius.
  • Treating theoretical results as production-ready. Every formula on this page is a planning estimate. Springback, material lot variation, and tooling wear all shift the real result — confirm with a first-article bend before locking a program.

90° bend deduction reference — mild steel, R = T

Bend deduction for a 90° bend at common mild-steel gauges, assuming inside radius equals material thickness (R = T — a standard air-bend rule of thumb) and K = 0.42 (mid-range mild steel/CRS). Computed from the formulas above; verify against your own tooling before locking a program.

Gauge Thickness (in) Thickness (mm) Bend deduction (in) Bend deduction (mm)
22 ga 0.0299 0.76 0.0529 1.34
20 ga 0.0359 0.91 0.0635 1.61
18 ga 0.0478 1.21 0.0846 2.15
16 ga 0.0598 1.52 0.1058 2.69
14 ga 0.0747 1.90 0.1322 3.36
12 ga 0.1046 2.66 0.1851 4.70
10 ga 0.1345 3.42 0.2380 6.05

Thickness values follow the Manufacturers' Standard Gauge for steel sheet. Bend deduction values are theoretical (formula-based); actual results depend on tooling, bend method, and material lot.

Frequently asked questions

What is the difference between bend allowance and bend deduction?
Bend allowance (BA) is the arc length of material consumed by the bend itself, measured along the neutral axis. Bend deduction (BD) is what you subtract from the sum of your flange lengths — measured to the outside mold line, the point where the flange faces would meet if extended to a sharp virtual corner — to get the flat pattern length. BD = 2 × setback − BA.
What K-factor should I use if I don't know my material or tooling?
Start with the typical range for your material family — about 0.33–0.38 for soft aluminum, 0.40–0.45 for mild steel or CRS, 0.45–0.50 for stainless — and use the midpoint as a first pass. These are starting values, not guarantees: K-factor shifts with tooling, bend method, and material lot, so confirm the real value on a test bend before locking a production program.
Does this calculator account for springback?
Not directly. Bend allowance and K-factor already bake in an empirical average for how material behaves through the bend, but the exact springback for your specific lot, thickness, and tooling can still shift the final angle by a degree or more. That's why every production program gets a first-article check before it's locked.
Why doesn't my flat pattern match my CAD software's flat pattern?
Most CAD packages default to a K-factor around 0.44 unless you've entered a bend table or material-specific K-factor for the part. If your material, thickness, or tooling differs from that default, the two won't agree until you set the same K-factor in both places.
What angle do I enter — the bend angle or its complement?
Enter A as the bend angle: the amount the material rotates through the bend, where 90° is a standard right-angle bend. This is the same convention used in the bend allowance formula's (π / 180) × A term.
Can I use this for aluminum or stainless, not just mild steel?
Yes — the bend allowance, setback, and bend deduction formulas are material-agnostic; only the K-factor changes. Choose the matching preset (soft aluminum, mild steel/CRS, or stainless) or enter your own test-bend-verified K-factor.

Ready to bend it for real?

This calculator gives you a theoretical flat pattern. Send us the part and we'll confirm it against real tooling with a first-article bend.

Request a quote Press brake capabilities