Bend allowance calculator

Work out a sheet metal bend in millimetres. Enter the thickness, the inside radius, the bend angle and a K-factor (or a Creo Y-factor, the DIN 6935 estimate, or your own test bend). You get the bend allowance, the outside and inside setback, the bend deduction and where the neutral axis sits. Then lay out a whole L, U, Z or hat profile and get its flat length and the bend-line positions on the blank. Free, no sign-up, runs in your browser.

It opens on a published worked example from press-brake maker Durma: 5 mm steel bent 90° over a 6 mm radius, K = 0.43, straight legs of 20 and 70 mm. Bend allowance 12.80 mm, flat length 102.80 mm. For springback and bending force, see the bending chapter of Skill-Lync's Manufacturing Processes book.

Units: mm and degrees · SOLIDWORKS, Creo, NX and Inventor terms · DIN 6935 · checked against 2D geometry (1294 checks at build) · Updated 22 Nov 2026

The test bend uses the thickness and radius above. Durma's generic starting values run from K = 0.33 to 0.50 (table below).

Profile and flat pattern

Flange 1 is on the left. "Up" turns the sheet anticlockwise as you walk along it. Every bend uses the radius, thickness and K-factor above; up to 8 flanges.

Bend allowance12.80 mmneutral radius 8.15 mm
Bend deduction9.20 mmvirtual sharp
OSSB / ISSB11.00 / 6.00mm, outside / inside setback
K-factor0.430Y = 0.675 · axis 2.15 mm in
Flat length102.80 mmΣBA 12.80 mm
Bends12 flanges
R 6.00 · A 90.0°T 5.00neutral axis dashed · to scale
B1flat length 102.80 mm
  • R/T = 1.20: inside radius at least the thickness.
BendAngle1st tangentCentre line2nd tangentBA
B190.0°20.0026.4032.8012.80
FlangeOutsideInsideFlange length
131.0026.0020.00
281.0076.0070.00

Bend-line positions are measured from the left end of the blank, in mm. The second table gives the same part dimensioned the three ways, so you can read a drawing in one convention and model it in another.

How to use the bend allowance calculator

  1. Enter the sheet. Thickness T and the inside bend radius R in mm. In air bending the radius comes from the die opening, not the punch, so use the radius your shop actually gets.
  2. Enter the angle. The bend angle A is how far the sheet turns: 90° makes a right angle. Drawings often give the included angle between the flanges instead; switch "Angles entered as" and the calculator uses 180° − your value.
  3. Choose the K-factor source. Type a K-factor, a Creo Y-factor, use the DIN 6935 estimate from R/T, or enter a test bend and the calculator works K out for you (the "reverse" calculation below).
  4. Lay out the profile. Pick L, U, Z or hat, or add flanges one by one with the angle and direction of each bend. Say how the drawing is dimensioned: outside, inside or flange lengths. You get the flat length, the bend lines on the blank and a CSV for the shop.

Bend allowance and bend deduction formulas

When sheet bends, the outside stretches and the inside is squeezed. Somewhere in between, a surface keeps its length: the neutral axis. It sits a distance t in from the inside face, and the K-factor is that distance as a fraction of the thickness. The bend allowance is the length of the neutral axis through the bend:

Drawings are usually dimensioned to the outside mold lines, where the flat faces would meet if the bend were sharp (the virtual sharp). The distance from the bend's tangent line to that point is the setback, and the bend deduction is what you subtract from the two outside dimensions:

For a single bend that gives the flat length either way: legs to the tangent plus BA, or outside dimensions minus BD. For a whole profile, each convention has its own sum:

Here d is each flange dimension as drawn. A U channel in 2 mm sheet, R = 3 mm, K = 0.38, outside 30 / 60 / 30 mm, has a flat length of 111.81 mm. Dimensioned inside it reads 28.0 / 56.0 / 28.0 mm, and as flange lengths 25.0 / 50.0 / 25.0 mm. Same blank, three drawings.

Worked example: Durma's 90° bend in 5 mm steel

Durma's bend allowance guide works a 90° air bend in medium steel: T = 5 mm, R = 6 mm, K = 0.43 (its table value for air bending with R between T and 3T), and straight legs of 20 mm and 70 mm measured to the tangent points. The calculator gives the same numbers:

  • BA = (π/2) × (6 + 0.43 × 5) = (π/2) × 8.15 = 12.80 mm (Durma: "BA ≈ 12.80 mm").
  • Flat length = 20 + 70 + 12.80 = 102.80 mm (Durma: 102.80 mm).
  • OSSB = tan 45° × (6 + 5) = 11.00 mm, so the outside dimensions are 31.00 and 81.00 mm, BD = 2 × 11.00 − 12.80 = 9.20 mm, and 31.00 + 81.00 − 9.20 = 102.80 mm again.

Skill-Lync's sheet metal course page uses a lighter case: 2 mm sheet, R = 2 mm, an L of 50 × 30 mm outside. With K = 0.33 the blank is 76.18 mm; with K = 0.5 it is 76.71 mm. That 0.53 mm is the cost of guessing K on one bend; a part with six bends multiplies it.

What K-factor should you use?

K depends on the radius-to-thickness ratio, the bending method and the material. Durma publishes these generic starting values and says they should be validated on your own press brake:

MethodR from 0 to TR from T to 3TR over 3T
Air bending0.33 / 0.38 / 0.400.40 / 0.43 / 0.450.50
Bottoming0.42 / 0.44 / 0.460.46 / 0.47 / 0.480.50
Coining0.38 / 0.41 / 0.440.44 / 0.46 / 0.470.50

Each cell lists soft / medium / hard material. Across a row K moves by up to 0.17; between materials in one cell, by 0.07 at most. Machinery's Handbook's 90° bend tables, as PTC reproduces them in Creo's help, group materials instead: K = 0.35 for soft brass and copper, 0.41 for hard brass, copper, soft steel and aluminium, and 0.45 for hard copper, bronze, cold-rolled steel and spring steel. The 0.446 default in Skill-Lync's K-factor blog sits next to that last value. None of these replaces a test bend on your material and tooling.

The DIN 6935 estimate

DIN 6935 gives a correction factor k from R/T, with the neutral fibre at k × T/2 from the inside. So the CAD K-factor is k/2:

R/T0.511.52345
k (DIN)0.4990.6500.7380.8010.8890.9511.000
K = k/20.2500.3250.3690.4000.4440.4760.500

These match Taupitz's published table (0.50, 0.65, 0.74, 0.80, 0.89, 0.95, 1.00) to two decimals. Its L-angle example, 50 × 40 mm outside in 2 mm sheet at R = 2 mm, has v = 3.84 mm and a blank of 86.16 mm; the calculator gives 86.16 mm. Below R/T = 0.5 the formula falls quickly (K = 0.150 at R/T = 0.2), so treat it as a rough guide there.

How to find the K-factor from a test bend

Cut a strip from the same sheet, measure its length L₀ and bend it on the tool you will use, to angle A at radius R. Measure the two outside legs a and b to the virtual sharp. Take away the straight parts and what is left is the bend allowance you actually got:

Example measurement: a 100.00 mm strip of 2 mm sheet bent 90° at R = 2 mm, both legs 51.80 mm. BA = 100 − 2 × (51.80 − 4.00) = 4.40 mm, so K = 0.401. Choose "A test bend" above to run your own. Measure with a vernier and use the longest strip the tool takes: an error of 0.05 mm in a or b moves K by about 0.016 here. If K comes out below 0 or above 0.5, recheck the measurement or the radius.

Bends past 90°: virtual sharp or tangent?

SOLIDWORKS measures bend deduction from the virtual sharp at every angle. Past 90° the virtual sharp moves away fast: for 2 mm sheet at R = 2 mm bent 135°, OSSB = tan 67.5° × 4 = 9.66 mm, and at 170° it is 45.7 mm. Many drawings therefore dimension such flanges to the tangent of the outer arc instead. DIN 6935 does this for opening angles up to 90° (bend angles of 90° and more), and SOLIDWORKS bend calculation tables have a "tangent length" switch for the same angle range:

On the 135° bend with K = 0.4, BD is 12.72 mm to the virtual sharp and 1.40 mm to the tangent. Pick the rule that matches the drawing in "Outside dims past 90°". Below 90° the two are the same. The calculator accepts bend angles between 0° and 180° and warns from 170°, where the part is close to a hem.

What SOLIDWORKS, NX, Creo and Inventor call it

CADTermWhat it is
SOLIDWORKSK-Factor, Bend Allowance, Bend Deduction, Bend Table, bend calculation tablesK = t/T, BA = π(R + KT)A/180; flat = A + B + BA or A + B − BD, with BD measured from the virtual sharp. Bend calculation tables can switch to tangent length by angle range.
Siemens NXNeutral FactorSiemens' NX blog describes it as the ratio between the sheet thickness and the neutral axis position, defaulting to 0.33 and settable from 0 to 1.
PTC CreoK factor, Y factorK = δ/T and Y = K × π/2; default Y = 0.50 (K = 0.318). Creo also ships bend tables.
Autodesk InventorUnfold rule: Linear, Bend Table, Custom EquationLinear applies one KFactor to every bend angle; Bend Table uses measured values with a backup KFactor.

So a SOLIDWORKS K-Factor and the K in an Inventor Linear unfold rule are the same number for the same part, NX's Neutral Factor does the same job on the same 0-to-1 scale, and a Creo Y-factor converts with Y = K × π/2. Bend tables in any of them override the formula with measured values, which is what you want once you have them.

Bend allowance and deduction table

For the sheet in the calculator (opening values: T = 5 mm, R = 6 mm, K = 0.43). It updates as you change the inputs; download it as CSV for a bend table.

Bend angleIncludedBASetbackISSBBD
15°165°2.131.450.790.76
30°150°4.272.951.611.63
45°135°6.404.562.492.71
60°120°8.536.353.464.17
75°105°10.678.444.606.21
90°90°12.8011.006.009.20
105°75°14.9414.347.8213.74
120°60°17.0719.0510.3921.04
135°45°19.2026.5614.4933.91
150°30°21.3441.0522.3960.77
165°15°23.4783.5545.57143.64

All values in mm. The setback and BD columns follow the outside-dimension rule you chose (virtual sharp unless you switched to tangent).

What this calculator does not cover

  • Springback and bending force: the angle the part opens up to after the punch lifts, and the press tonnage. Both are in the bending chapter of the Manufacturing Processes book, with interactive sliders.
  • Material minimum bend radii and hole-to-bend distances: take these from your supplier or a DFM guide; the DFM checklist covers bend radius and hole-to-bend rules.
  • Hems, jogs, offsets and rolled shapes, which most CAD tools handle with their own rules or tables.
  • Different radii per bend: every bend here uses one R, T and K. Work a mixed part bend by bend with the single-bend results.
  • Inch units and gauge numbers: the calculator works in mm only. Gauge thickness depends on the material, so convert to mm first.
Learn sheet metal design

Flat patterns, bend tables and K-factors are everyday work for sheet metal and BIW designers. Skill-Lync's sheet metal courses teach the full workflow in Siemens NX and CATIA V5.

Frequently asked questions

What is the bend allowance formula?

Bend allowance is the neutral axis length through the bend: BA = (π × A/180) × (R + K × T), where A is the bend angle in degrees, R the inside radius, T the thickness and K the K-factor. Durma's 5 mm steel bent 90° at R 6 mm with K = 0.43 gives BA = 12.80 mm.

What is the difference between bend allowance and bend deduction?

Bend allowance is added to the straight flange lengths; bend deduction is subtracted from the outside (mold-line) dimensions. They describe the same blank: BD = 2 × OSSB − BA, with OSSB = tan(A/2) × (R + T). For Durma's 90° example, OSSB = 11.00 mm and BD = 9.20 mm, so 31 + 81 − 9.20 = 102.80 mm.

What is the K-factor for copper?

There is no single value. Machinery's Handbook bend tables, as reproduced in PTC Creo's help, put soft copper with soft brass at K = 0.35 and hard copper with bronze and cold-rolled steel at 0.45 for 90° bends. The radius-to-thickness ratio and the bending method move K as much, so measure it with a test bend.

What K-factor should I use?

Start from your CAD's default or a table, then measure. Durma's generic starting values run from 0.33 (soft material, air bending, R up to T) to 0.50 once R exceeds 3T, for air bending, bottoming and coining alike. Creo's default Y-factor of 0.50 is K = 0.318; Siemens NX's neutral factor defaults to 0.33.

How do I find the K-factor from a test bend?

Measure a strip's length L₀, bend it on your tool to angle A and measure both outside legs a and b. Then BA = L₀ − (a − OSSB) − (b − OSSB) and K = (BA/A_rad − R)/T. A 100 mm strip of 2 mm sheet bent 90° at R 2 with 51.80 mm legs gives K = 0.401.

What is the Y-factor in Creo?

PTC Creo describes the neutral axis with a K factor and a Y factor, related by Y = K × π/2. Creo's documented default is Y = 0.50, which is K = 0.318. You can enter either in Creo; this calculator converts a Y-factor to K with K = 2Y/π and shows both.

Related on Skill-Lync

Sources

  • Durma, "Bend Allowance Formula: Calculation, K-Factor & Worked Examples": the worked example (90° air bend in steel, R 6 mm, T 5 mm, K 0.43, straight sections "20 mm and 70 mm, measured to the tangent points", "BA ≈ 12.80 mm", flat 102.80 mm) and the "generic K-factor starting values" by method and R/T. Read 22 Nov 2026.
  • Dassault Systèmes, SOLIDWORKS 2022 help: K-Factor ("a ratio that represents the location of the neutral sheet with respect to the thickness", "BA=pi(R + KT) A/180"); Bend Allowance and Bend Deduction ("You must measure the bend deduction (BD) from the virtual sharp"; "the bend deduction is the difference between the bend allowance and twice the outside setback"); Bend Calculation Tables ("virtual sharp or tangent length", ß = aperture angle, "0 <= ß <= 90 Tangent length = Yes"). Read 22 Nov 2026.
  • Dassault Systèmes, SOLIDWORKS DFMXpress: bend radius rule: "the inside bend radius should exceed the thickness of the material". Read 22 Nov 2026.
  • PTC, Creo help: About Y factor and K factor ("Y factor = K factor * (Π/2)", "The default value for Y factor is 0.50"); About Bend Tables (three 90° tables "from the Machinery's Handbook, 28th Edition": soft brass, copper K 0.35; hard brass, copper, soft steel, aluminum K 0.41; hard copper, bronze, cold rolled steel, spring steel K 0.45). Read 22 Nov 2026.
  • Siemens, NX Tips and Tricks: Sheet Metal (21 Mar 2024): bend parameters have "an option to set a neutral factor", which "defaults to 0.33, but can be set anywhere between 0 and 1". Read 22 Nov 2026.
  • Autodesk, Inventor 2025 help: To Add, Edit, or Sync a Sheet Metal Unfold Rule: Linear "unfolds sheet metal part using a KFactor that is applied uniformly to all bend angles"; Bend Table and Custom Equation with a Backup KFactor. Read 22 Nov 2026.
  • Taupitz, "Gestreckte Länge beim Biegen von Blechen berechnen" (DIN 6935): "k = 0,65 + 0,5 · log10(Ri / t)", k = 1 from Ri/t = 5, "K-Faktor (CAD) = k (DIN 6935) / 2", the v formulas by opening angle (2(Ri + t) up to 90°, the tan form from 90° to 165°), the k table and the L-angle examples (50 × 40 mm, t 2, Ri 2: v −3.84, L 86.16 mm; 120°: L 88.16 mm; t 3, Ri 3, 100 × 60: L 154.24 mm). Read 22 Nov 2026.
  • Skill-Lync, scripts/verify/bend_allowance.py: builds every profile as 2D geometry (mid-line arcs and flanges, both faces), measures outside and inside dimensions from face-line intersections, finds flange lengths by iteration, integrates the neutral line numerically, finds the reverse K by bisection and rebuilds the published DIN and Durma examples. The page compares 1294 numbers with it when it is built.
Free counselling

From a flat pattern to a sheet metal design career.

Sheet metal and BIW design roles at OEMs and engineering services firms ask for exactly this: parts that unfold right the first time. A Skill-Lync counsellor can tell you which course fits where you are now.

Talk to a course counsellor

Free. We call you back, usually the same day.

By submitting you agree to our Terms and Privacy Policy.

Talk to a career counsellor

Talk to a career counsellor

Free 20-minute call. We'll map the right course to where you want to work.

By submitting you agree to our Terms and Privacy Policy.