K-Factor Calculator uses $BA=A_{rad}(R+K\times T)$ to find sheet metal bend allowance, bend deduction, setbacks, neutral axis depth, and radius from thickness, inside radius, angle, and K-factor.
Flat Pattern Development Starts Here — Not at the Press Brake
A flat pattern that’s wrong by half a millimeter will be wrong on every part you cut from it. The K-Factor is the single variable that determines where the neutral axis sits inside the material during a bend — that imaginary line through the cross-section that neither stretches nor compresses. Get it right and your flanges land where the print says they should. Guess it, and you’re trimming finished parts.
This calculator takes the K-Factor as an input, not something it solves for. If you’re here to find your material’s K-Factor from test bends, you’ll need to measure the actual flat pattern length of a finished bend and back-calculate. What this tool does is take the K-Factor you’ve already determined — or are using from a material table — and produce the complete bend geometry: Bend Allowance, Bend Deduction, both setback values, neutral axis depth, and the R/T severity ratio that tells you whether your inside radius is safe for that material.
The Four Numbers That Define a Bend
Bend Allowance — What the Hero Display Shows
Bend Allowance (BA) is the arc length that the neutral axis travels through the bend. It’s not the outside of the curve and it’s not the inside — it’s the specific arc at depth K × T from the inside surface. The formula is straightforward once you accept that geometry: BA = angle_in_radians × (R + K × T). The radius used isn’t the inside bend radius R — it’s the neutral axis radius, which is always R + K×T. A K of 0.44 on 0.125-inch material puts the neutral axis at 0.44 × 0.125 = 0.055 inches from the inside surface, and that’s the radius the arc length formula uses.
Bend Deduction — What You Subtract in CAD
Bend Deduction (BD) is what most CAD flat pattern tools actually ask for. It’s the amount you subtract from the sum of outside flange dimensions to get the flat blank length. The formula the calculator uses is BD = (2 × OSSB) − BA, where OSSB is the Outside Setback. On a 90° bend, the Outside Setback equals (R + T) × tan(45°) = R + T. For non-right angles, the tangent of half the bend angle scales both setback values — which is why the tan-half-angle ratio appears as its own output in Card 2.
Setbacks — Inside vs. Outside
The Outside Setback (OSSB) is the distance from the bend tangent line to the projected sharp outside corner of the material. The Inside Setback (ISSB) is the same measurement taken from the inside corner. Their difference is exactly the material thickness at right angles. These matter for minimum flange length — if your flange dimension is shorter than the OSSB, the flat pattern will require a negative material length, which is physically impossible. The calculator surfaces both values so you can catch that condition before it reaches the shop floor.
Neutral Axis Depth and Y-Factor
The neutral axis depth is simply K × T — the absolute position of the neutral axis measured from the inner surface. The “Offset From Mid-Thickness” shown in Card 3 is how far that position is from the geometric center of the material (T/2). At K = 0.5, the neutral axis sits exactly at mid-thickness and the offset is zero — the theoretical upper bound for standard bending. The Y-Factor displayed alongside it is K × π/2, an alternative representation used in some European DIN-based design tables and certain CAD systems that use Y-Factor instead of K-Factor in their bend table parameters.
When the Bend Severity Ratio Matters
The calculator computes R/T — the ratio of inside bend radius to material thickness — and displays it in Card 4 under “Radius / Thickness.” When that ratio drops below 1.0, the alert switches to a warning about fracture risk. That threshold isn’t arbitrary.
A bend radius smaller than the material thickness means the outer fiber of the material is being stretched beyond what most ductile sheet metals can sustain without cracking. Work-hardened alloys and thicker plate are more susceptible; soft annealed material can occasionally tolerate it.
But below R/T = 1, you’re in territory where the geometry is mathematically valid but practically risky, and a qualified material engineer or press brake operator should confirm the setup before cutting blanks.
A second alert condition: K-Factors above 0.5 also trigger a warning. Standard air bending on mild steel typically runs between 0.38 and 0.44. Values above 0.5 usually indicate coining, extreme bottoming, or special tooling — conditions where the material is forced past its neutral state. Entering K = 0.6 won’t break the calculation, but the alert flags it so you’re not using an unusual value by accident.
Worked Example: Instrument Panel Bracket, 16 ga Cold-Rolled Steel
An enclosure shop is making mounting brackets from 16-gauge cold-rolled steel, which measures 0.060 inches thick on their incoming material inspection. The design calls for a 90° bend with a 0.060-inch inside radius — a 1:1 R/T ratio, right on the edge of the severity threshold. They’re using standard air bending on a 28-ton press brake, so K = 0.44 from their established material table.
Entering T = 0.060, R = 0.060, angle = 90°, K = 0.44 gives: BA = (π/2) × (0.060 + 0.44 × 0.060) = 1.5708 × 0.0864 = 0.1357 inches. The Outside Setback works out to (0.060 + 0.060) × tan(45°) = 0.120 inches. Bend Deduction is (2 × 0.120) − 0.1357 = 0.1043 inches. The severity ratio reads exactly 1.00 — the alert doesn’t fire, but it’s close enough that the operator decides to bump the radius to 0.090 inches on the second batch to build in margin. Rerunning with R = 0.090 drops the BD slightly to 0.0763 inches and raises the severity to 1.50, clearing the warning comfortably.
The flat pattern width for a bracket with two 1.5-inch flanges would be: 1.5 + 1.5 − BD = 3.0 − 0.1043 = 2.8957 inches, rounded to 2.896 on the DXF. That’s what goes to the laser nest.
Frequently Asked Questions
Why does the calculator reject K-Factor values of 1.0 or higher?
K = 1.0 would place the neutral axis at the outer surface of the material, which is physically impossible — the outer fiber is the most stretched point in any bend, not a zero-strain location. The tool enforces a strict upper limit of less than 1.0. Similarly, K = 0 would place the neutral axis at the inside surface, which is also unrealistic. Valid K-Factor inputs run from just above 0 to just below 1, with practical sheet metal values almost always between 0.25 and 0.50.
The calculator accepts 179.9° but not 180°. What happens at exactly 180°?
A 180° bend — a hemmed edge — would require computing the tangent of 90°, which is mathematically undefined (approaches infinity). The setback and bend deduction formulas both use tan(angle/2), so any angle at or above 180° breaks the formula entirely. The input field enforces a maximum of 179.9°. If you’re designing a hem, the flat pattern calculation works differently and isn’t what this tool is built for.
When I switch between US Customary and Metric, my numbers don’t convert. Is that a bug?
It’s intentional design, and it’s worth understanding. The unit system toggle changes the label on the result outputs (in vs. mm) but does not convert the numbers you’ve typed. If you enter 3.175 in metric mode and switch to US, the field still reads 3.175 but is now being interpreted and labeled as 3.175 inches — a very different physical dimension. Enter your values in the unit system you intend to use from the start. The toggle is there to match result labels to your working units, not to perform dimensional conversion between systems.
What’s the difference between the Inside Setback and Outside Setback, and when does each one matter?
The Outside Setback (OSSB) is measured to the projected sharp corner on the outside of the bend — the phantom corner that would exist if the bend had zero radius. Bend Deduction is derived from OSSB, so it directly affects your flat pattern length calculation. The Inside Setback (ISSB) is the same measurement taken to the inside sharp corner. The practical use of ISSB is checking minimum flange length: your designed flange must be at least as long as the OSSB, or the flat blank math produces a negative dimension. The ISSB figure is useful when back-calculating from an existing part rather than designing from scratch.
The default K-Factor is 0.44. Where does that number come from?
It’s a widely used industry convention for mild cold-rolled steel with standard air bending tooling — not a value mandated by any single standard, but one that appears consistently across fabrication shop tables, press brake manufacturer documentation, and sheet metal design references. Softer materials like aluminum in the 5052 alloy tend to run 0.38–0.41. Harder or pre-hardened materials may use 0.45–0.48. The only reliable way to know your actual K-Factor is to bend a test piece, measure the resulting flat pattern length, and solve for K from the BA formula. The default 0.44 is a starting point, not a substitute for material-specific data on precision work.