Article — K-Factor Calculator
K-factor calculator: bend allowance and flat-pattern math for sheet metal
A K-factor calculator returns the bend allowance, outside setback, and bend deduction for a sheet metal bend, given material thickness, inside bend radius, bend angle, and K-factor. K-factor is the position of the neutral axis as a fraction of material thickness — typically 0.33 for soft brass, 0.41 for mild steel with r≥t, 0.42 for aluminum, up to 0.50 theoretical max. For 2 mm steel at 90° with 3 mm inside radius and K = 0.41, the bend allowance is 6.00 mm — the arc length on the neutral axis that determines the flat blank length.
Sheet metal layout is unforgiving math: a 0.5 mm error in bend allowance, multiplied across four bends in a box, leaves the corners 2 mm out of square. CAD software does the calculation automatically once K-factor is set, but the value depends on material, thickness, radius, and tooling. The K in a published table is a starting estimate. Production parts need a calibrated K from a test bend.
What is K-factor in sheet metal
When sheet metal bends, the outside surface stretches and the inside surface compresses. Somewhere in the middle is the neutral axis — the layer of material that neither stretches nor compresses. K-factor is the position of this neutral axis as a fraction of material thickness, measured from the inside surface.
BA = (π/180) × θ × (r + K·t) bend allowanceOSSB = tan(θ/2) × (r + t) outside setbackBD = 2·OSSB − BA bend deductionL_blank = L⊂₁ + L⊂₂ − BD flat patternK = 0 places the neutral axis at the inside surface; K = 0.5 places it dead center. Values above 0.5 are physically impossible because no material can stretch more on the inside than it does on the outside. Real-world K values for common materials and tooling run 0.30 to 0.48, with steel and aluminum hovering near 0.40 to 0.45.
K-factor and bend allowance formulas
Bend allowance (BA) is the arc length on the neutral axis, in the same units as your thickness and radius. The formula is BA = (π/180) × bend angle × (inside radius + K × thickness). For 2 mm steel at 90° with r = 3 mm and K = 0.41: BA = 1.5708 × (3 + 0.82) = 6.00 mm.
Outside setback (OSSB) is the distance from the bend line to the apex of the bend on the outside surface. For 90° bends, OSSB = r + t. For other angles, OSSB = tan(angle/2) × (r + t). Bend deduction (BD) is the most useful number for layout: BD = 2 × OSSB − BA. For the example: BD = 2 × 5 − 6 = 4 mm.
K-factor by material and tooling
Material affects K mostly through its ductility. Soft, ductile materials (annealed brass, copper) stretch more easily on the outside, pulling the neutral axis toward the inside — lower K. Hard, stiff materials (cold-rolled steel, hardened aluminum) resist outer stretching, pushing the neutral axis toward the middle — higher K.
The often-quoted K = 0.33 number comes from soft brass under air bending and is wrong for almost everything else. It got copied into early CAD documentation and stuck around as a default. Mild steel under typical air bending is closer to K = 0.41 to 0.44. Picking 0.33 for steel produces flat patterns that are 5 to 10% too long — visible misalignment in the final part. Always pick the value that matches your material and tooling, not the textbook default.
Bend radius matters too. When the inside radius is smaller than the material thickness (r < t), the inside material gets crushed and the neutral axis shifts toward the inside (lower K, 0.30 to 0.38). When the radius is larger (r > 2t), the neutral axis stays close to center (higher K, 0.43 to 0.48).
K-factor for air, bottom, and coin bending
Three press-brake bending methods produce different K-factors. Air bending uses a punch that does not bottom out in the die — the angle is set by punch depth. K-factor ranges 0.38 to 0.45 with significant variation by die opening width. Bottoming pushes the material to the die bottom for a more consistent angle; K typically lands 0.40 to 0.42.
Coining uses high tonnage to fully compress the material in the die, plastically deforming the bend zone. K reaches 0.42 to 0.50, near the theoretical maximum. Coining is used for parts that require dimensional precision and high spring-back resistance, at the cost of higher tonnage and tool wear.
Calibrating K-factor from a test bend
For production parts, do not trust handbook K-factors. Bend a coupon, measure the result, back-solve K. The procedure: cut a known blank length, bend it 90° in your tooling, measure the legs (from the outside corner of the bend to the end of each flange).
- Cut a blank = known length, typically 100 to 200 mm depending on tooling
- Bend at 90° = same radius and tooling as production
- Measure both legs = outside corner to end, sum the two
- Solve BA = blank length minus sum of legs
- Solve K = BA × 180 / (π × angle × (r + t/2)), then refine
- Average three bends = lot-to-lot variation matters
Bend deduction vs bend allowance
Bend allowance and bend deduction describe the same physical bend but from different layout perspectives. Bend allowance is the arc length you add when developing the bend zone separately from the legs. Bend deduction is the amount you subtract from the sum of leg lengths to get the flat blank length.
Most CAD systems and shop drawings use bend deduction because the calculation is more direct: measure the legs from the bend apex (where the outside surfaces would meet if extended), sum them, subtract BD, you get the flat length. Bend allowance is more useful when working with arc-development geometry directly.
Flat-pattern math for multi-bend parts
For a part with multiple bends, sum all leg lengths (measured to bend apexes) and subtract each bend’s BD. A four-sided box with each side 100 mm has 8 legs of 50 mm each plus four bends. Total leg sum: 400 mm. Subtract 4 × 4 mm = 16 mm. Flat blank: 384 mm.
When mixing bend angles (some 90° with some 45°), each bend has its own BD because OSSB depends on angle. Always compute per-bend, then sum. A flat pattern with 90° bends at the corners and 45° bends in chamfered edges uses two different BDs — do not average them.
Common K-factor mistakes
Using the default K = 0.33 for steel is the most common mistake, traced back to early CAD documentation. The right value for mild steel under air bending with r ≥ t is 0.41 to 0.44. Using 0.33 produces blanks that are 4 to 6% too long — the legs come out long, and you trim every part after bending.
Forgetting tooling-specific calibration is the second mistake. A K-factor that works on one press brake with one die set does not transfer cleanly to another. Different die widths, different punch radii, different back-gauge accuracy — each shifts K by 0.02 to 0.05. Calibrate per-machine, per-tool combination.
K-factor predicts the bend allowance for a finished bend angle. Springback is the additional bend angle the material recoils after releasing pressure — you overbend by a few degrees to land at the target. Both effects depend on material and tooling, but they correct different things. Adjusting K to compensate for springback produces a flat pattern that is right at the wrong target angle.
Mixing units within a calculation is the third mistake. The K-factor formula is dimensionally consistent only when thickness, radius, and bend allowance use the same unit. Common mismatches: thickness in mm but radius in inches. Convert before calculating; do not mix mid-equation.