Sheet Metal Bend Allowance Calculator — K-Factor, Bend Deduction & Developed Length
Calculate sheet metal bend allowance, bend deduction, and flat pattern developed length. Includes K-factor for material, thickness, and bend radius combinations.
Quick Answer
For a 2mm mild steel sheet, 90° bend, inside radius 2mm, K-factor 0.38: Bend Allowance = 3.72 mm, Bend Deduction = 4.28 mm. For a bracket with two 90° flanges of 30mm and 40mm: Flat Pattern Length = 30 + 40 − 4.28 = 65.72 mm. Without bend deduction, you’d cut 70mm — 4.3mm too long.
Why Bend Allowance Matters to the Tenth of a Millimeter
Sheet metal bends stretch the outside and compress the inside. The neutral axis shifts inward — the flat pattern is shorter than the sum of flange lengths. Getting this wrong means parts don’t fit.
1. K-Factor = t_neutral / t
The distance from the inside bend surface to the neutral axis, divided by material thickness. K=0.5 means the neutral axis is at the mid-thickness — true for pure elastic bending only. Real K-factors: 0.33-0.38 for most steels (neutral shifts inward due to plastic compression). Larger bend radii → higher K (closer to 0.5).
2. Bend Allowance (BA)
BA = (π/180) × (R + K×t) × A, where R=inside radius, t=thickness, A=bend angle. This is the arc length of the neutral axis through the bend. BA is added to flange lengths to get the flat pattern.
3. Bend Deduction (BD)
BD = 2 × OSSB − BA, where OSSB = outside setback = (R+t)×tan(A/2). BD is the amount to subtract from the sum of outside flange lengths. Most shops use BD tables because you measure outside dimensions on the formed part — subtract BD to get flat.
Common Mistakes
- Using K=0.5 for all materials — K=0.5 is pure elastic bending and wrong for most production bends. Mild steel (air bending): K≈0.33-0.38. Stainless: K≈0.35-0.40. Aluminum 5052: K≈0.33-0.38. Soft/bright aluminum: K≈0.40-0.45. Wrong K-factor gives length errors of 0.5-1.5mm per bend — a 4-bend part is 2-6mm off.
- Not accounting for bend radius variation — Air bending radius is NOT the punch radius — it’s determined by die opening: R ≈ V/8 for steel, V/6 for aluminum. A 2mm punch in a 16mm V-die produces ~2mm inside radius. Bottom bending uses the punch radius directly — know your process.
- Assuming bend deduction from one machine applies to another — Each press brake has different tonnage, deflection, and springback characteristics. Bend deduction values are machine-specific. Don’t share BD tables between machines without verification — the first part will be wrong.
- Forgetting about grain direction — Bending across grain requires 15-20% larger inside radius than bending with grain to avoid cracking. Grain direction also shifts K-factor slightly. Aerospace and medical parts often specify grain direction on the flat pattern.
- Not compensating for bend sequence — The first bend is “clean” (no interference). Subsequent bends may hit the tooling or previously formed flanges. A 2-bend Z-bracket needs sequence planning: bend the smaller flange first, then the larger flange has clearance. Sequence affects gauge point locations and achievable accuracy.
Frequently Asked Questions
What is the difference between bend allowance and bend deduction?
Bend Allowance (BA): length of the neutral axis arc through the bend — added to inside flange lengths. Bend Deduction (BD): amount subtracted from sum of outside flange lengths. BA = added, BD = subtracted. Most shops use BD because they measure outside-to-outside on the formed part. Both give the same flat pattern length.
How do I determine the K-factor for my material?
Test bend method: (1) Cut a known-length strip, (2) Bend 90° at your production radius, (3) Measure the two flange lengths, (4) Back-calculate: K = (BA × 180/(π×A) − R) / t, where BA = L_flat − L₁ − L₂ + BA (iterative). Or: use known values from bend allowance tables. BendTech, SolidWorks, and Inventor have built-in K-factor libraries.
What is the minimum bend radius for different materials?
Mild steel: 1× thickness (softer grades bend to 0.5×). Stainless 304: 1× thickness (work-hardens, springback is high). Aluminum 5052-H32: 1× thickness. Aluminum 6061-T6: 1.5-2× thickness (brittle — cracks easily). Copper: 0.5-1× thickness (ductile). Rule: R_min = t/(2r − 1) where r = reduction of area. When in doubt, bend across the grain with a larger radius.
How does springback affect bend allowance?
Springback opens the bend angle — a 90° punch produces an 88-92° bend, depending on material. Springback compensation: over-bend by the springback angle. Springback does NOT change bend allowance significantly (the arc length stays nearly the same) — it just changes the angle. Compensate angle; BA stays the same.
What about hemming and flattening?
Hem (180° bend): flat pattern includes hem allowance = 1.5× to 2.5× material thickness (depends on hem type). Teardrop hem (open): allow ~2×t. Flattened/closed hem: allow ~1.5×t — the material thinning in the hem compensates for the extra length. Hemming is specialty — verify with test bends.
How does material thickness tolerance affect flat pattern?
Commercial tolerance: ±0.08mm for 1mm sheet, ±0.13mm for 3mm. BA changes ~0.03mm per 0.01mm thickness change. Over 10 bends, thickness tolerance alone can shift flat pattern ±1-2mm. For tight-tolerance parts: measure actual thickness and adjust K-factor, or use gauge material (tighter tolerance) and formed reference dimensions.
Should I design in the formed or flat state?
Design in the formed state — that’s what fits the assembly. The flat pattern is a manufacturing intermediate. CAD transforms from formed to flat using K-factor. Exception: blanking dies — design the flat because the formed shape comes from the die geometry.
How many bends before I need to worry about cumulative error?
Each bend contributes ±0.1-0.3mm of position error (depending on press brake accuracy, material variation, and operator skill). 3 bends: manageable. 6 bends: tolerance stack becomes significant. 10+ bends: consider GD&T with profile tolerancing, not ± linear dimensions. For multi-bend parts, our Tolerance Stack-Up Calculator helps analyze cumulative error.