Bend Allowance and K-Factor Explained
How to calculate flat pattern length for sheet metal bends, with a worked example and typical K-factor values
Bend allowance is the length of material consumed by a bend, and the K-factor is the ratio that locates the neutral axis inside the bend so a flat pattern can be calculated before cutting. Get either wrong and a bent bracket comes out 2-5 mm short or long on its flange, which is the most common rejection cause CutLinq sees on customer-supplied flat patterns.
This page gives the standard formulas, typical K-factor values by material and bend radius, and a worked example so you can check your own flat pattern or your CAD software's unfold before sending a DXF for quoting.
The neutral axis and why K-factor exists
When sheet metal bends, the outer surface stretches and the inner surface compresses. Somewhere through the thickness there is a neutral axis that neither stretches nor compresses; K-factor is the position of that axis expressed as a fraction of thickness measured from the inside surface (K = t_neutral / t_total). A K-factor of 0.44 means the neutral axis sits 44% of the way through the material from the inside face.
K-factor is not a fixed material constant. It depends on bend radius relative to thickness, on bend angle, and on the process (air bending versus bottoming or coining), so software defaults are a starting point, not a guarantee.
| Inside radius / thickness | Typical K-factor (air bend) | Notes |
|---|---|---|
| R < 1x t (sharp bend) | 0.33-0.38 | More material compression |
| R = 1x t to 2x t | 0.40-0.44 | Most common range for sheet 1-6 mm |
| R = 2x t to 4x t | 0.44-0.48 | Larger, gentler bends |
| R > 4x t | 0.48-0.50 | Approaches simple mid-plane assumption |
Formulas: bend allowance and bend deduction
Bend allowance (BA) is the arc length of the neutral axis through the bend: BA = angle_radians x (R + K x t), where R is the inside bend radius, t is thickness and angle is the bend angle in radians (angle_degrees x pi / 180). Flat pattern length = sum of flange lengths (measured to the tangent point) + BA for each bend.
Many CAM systems instead use bend deduction (BD), which is subtracted from the sum of the outside flange dimensions: BD = 2 x (R + t) x tan(angle/2) - BA. Bend deduction is more convenient when flanges are dimensioned to the outside of the part, which is how most drawings are toleranced.
| Term | Formula | Used when |
|---|---|---|
| Bend allowance (BA) | θ(rad) x (R + K·t) | Flanges measured to bend tangent |
| Bend deduction (BD) | 2(R+t)·tan(θ/2) - BA | Flanges measured to outside corner |
| Setback (SB) | (R+t)·tan(θ/2) | Locating the bend line from a corner |
Worked example: 90° bend in 3 mm S235JR
Part: an L-bracket, 3 mm S235JR, inside radius 3 mm (R = t, a typical air-bend radius), 90° bend, flange legs 40 mm and 60 mm measured to the outside corner.
Step 1: K-factor for R = 1t is about 0.42 (from the table). Step 2: BA = (90 x pi/180) x (3 + 0.42 x 3) = 1.5708 x 4.26 = 6.69 mm. Step 3: BD = 2 x (3+3) x tan(45°) - 6.69 = 12 - 6.69 = 5.31 mm. Step 4: flat length = 40 + 60 - 5.31 = 94.69 mm. Cut the blank at approximately 94.7 mm before bending.
Where K-factor tables go wrong
Software default K-factors (commonly 0.44 for all bends) are only accurate near R = 2t. For sharp radii under 1x thickness, using 0.44 overestimates the flat length and the flange comes out short after bending. For stainless steel, which work-hardens more than mild steel, K-factor runs 0.02-0.03 lower than the equivalent mild steel bend at the same radius because the material resists compression on the inside face more.
For critical assemblies, CutLinq recommends bending a first-article sample and adjusting the flat pattern by measurement rather than trusting a single K-factor for the whole range of bends on a part.
Design tips
- Use inside radius equal to material thickness as a default for mild steel; it gives a predictable K-factor near 0.42-0.44.
- For stainless steel, use inside radius of 1.0-1.5x thickness to reduce cracking risk on the outer fiber.
- Never specify a bend radius smaller than the material thickness for aluminium 5754 or 6061-T6; it will crack.
- Dimension flanges to the outside corner on drawings; it maps directly to bend deduction and avoids ambiguity.
- State the K-factor or bend allowance table you used on the drawing if it differs from CutLinq's default, so first-article checks match.
- For a part with many different bend radii, request a first-article sample before committing to a production run.
- Add ±0.5° angle tolerance and ±0.3 mm flange tolerance as a realistic press brake capability, not a stated zero tolerance.
Applications
| Industry | Example parts | Typical material |
|---|---|---|
| Sheet metal enclosures | Chassis, covers, brackets | DC01, S235JR 1-3 mm |
| HVAC ductwork | Transition pieces, plenum boxes | Galvanised DX51D 0.6-1.5 mm |
| Machine guarding | Bent panels, access doors | S235JR 1.5-3 mm |
| Signage frames | Cabinet returns, mounting brackets | Aluminium 5754, stainless 304 |
| Furniture and fit-out | Legs, brackets, shelving | DC01, 304 stainless 1-2 mm |
Pricing and lead time
Bending cost is driven by the number of bends and setups (each new bend orientation needs a tool change or a re-clamp), by part length (parts over about 2 metres may need a second operator or a special tool), and by tolerance (angle tolerances tighter than ±0.5° require slower, checked bending). A DXF with correct flat pattern and clearly marked bend lines avoids a design review delay; expect laser-cut and bent brackets in 3-5 working days across Egypt, the UAE and Saudi Arabia.
Frequently asked questions
Yes, send a STEP file of the bent part and we unfold it using our own K-factor tables rather than trusting the K-factor baked into your CAD software, which reduces first-article mismatches.
Upload your flat DXF or bent STEP file, and receive a binding quote within 12 hours.