The K-factor is the position of the neutral axis inside a bend, expressed as a fraction of the sheet thickness. For most sheet metal it sits between 0.3 and 0.5, and 0.4 to 0.45 is common for air-bent mild steel at a radius about equal to thickness.
Why care? Your CAD program uses the K-factor to unfold a bent part into a flat blank. Use the wrong one and every flange comes out a fraction of a millimetre off, which adds up quickly on a box with six bends. Below we cover what the K-factor actually describes, the bend allowance formula, a full worked example, and why the shop's number should win.
The neutral axis, in plain terms
Bend a strip of metal and the outside stretches while the inside squashes. Somewhere between the two faces is a layer that does neither. It stays exactly the length it was when the sheet was flat. That layer is the neutral axis.
If metal bent perfectly evenly, the neutral axis would sit right in the middle of the thickness, and the K-factor would be 0.5. In practice, the inside compresses less readily than the outside stretches, so the neutral axis shifts towards the inside of the bend. That's why real K-factors are usually below 0.5.
The K-factor is just that position as a ratio:
- K = 0 means the neutral axis is on the inside face.
- K = 0.5 means it's exactly in the middle.
- K = 0.44 means it's 44% of the way from the inside face to the outside face.
Because the neutral axis doesn't change length, it's the line you measure to work out how long the flat blank must be.
The bend allowance formula
Bend allowance (BA) is the length of the neutral axis through the curved part of the bend. Think of it as how much flat sheet the bend uses up.
The formula is:
BA = A × π/180 × (R + K × T)
Where:
- A is the bend angle in degrees, measured from flat (a 90° bend is 90)
- R is the inside bend radius in mm
- K is the K-factor
- T is the material thickness in mm
The A × π/180 part converts the angle to radians. The (R + K × T) part is the radius of the neutral axis. Multiply them and you get the arc length. That's all it is.
Worked example: a 2 mm mild steel L-bracket
Here's a simple bracket: 2 mm mild steel, one 90° bend, outside dimensions of 50 mm and 30 mm, inside radius 2 mm. We'll use K = 0.44.
Step 1: the bend allowance.
- Neutral axis radius: R + K × T = 2 + 0.44 × 2 = 2 + 0.88 = 2.88 mm
- Angle in radians: 90 × π/180 = 1.5708
- BA = 1.5708 × 2.88 = 4.52 mm
Step 2: the straight sections. The outside dimensions run to an imaginary sharp corner. The curve starts R + T = 4 mm back from that corner on each leg. So the flat, straight parts are:
- Long leg: 50 − 4 = 46 mm
- Short leg: 30 − 4 = 26 mm
Step 3: add them up. Flat length = 46 + 26 + 4.52 = 76.52 mm.
You can also get there with a bend deduction, which is what many shops use day to day. The outside setback for a 90° bend is tan(45°) × (R + T) = 1 × 4 = 4 mm. Bend deduction = 2 × 4 − 4.52 = 3.48 mm. Flat length = 50 + 30 − 3.48 = 76.52 mm. Same answer, which is a good sign the arithmetic is right.
How much the K-factor changes the answer
Same bracket, three different K-factors:
| K-factor | Neutral axis radius | Bend allowance | Flat length |
|---|---|---|---|
| 0.33 | 2.66 mm | 4.18 mm | 76.18 mm |
| 0.44 | 2.88 mm | 4.52 mm | 76.52 mm |
| 0.50 | 3.00 mm | 4.71 mm | 76.71 mm |
That's about half a millimetre between the extremes on one bend. On its own, small. On a hat section with four bends along its width, the error stacks up to around 2 mm, which is enough to make a lid not fit or a bolt pattern miss.
The radius matters just as much. The same maths with a 3 mm radius instead of 2 mm adds another 1.57 mm to the bend allowance. If your CAD radius doesn't match the radius the press brake produces, the flat pattern is off before the K-factor even enters into it. Our guide to sheet metal bend radius explains how that radius is set by the tooling.
Why there's no universal K-factor
You'll find tables online listing K-factors for steel, stainless, and aluminium. Treat them as starting points. The real value depends on:
- The material and its hardness. Stronger material shifts the neutral axis differently.
- The radius-to-thickness ratio. Tight bends tend to have a lower K-factor; large, gentle bends move towards 0.5.
- The bending method and tooling. Air bending, bottoming, and coining all behave differently, and the die opening changes the radius.
- The batch of sheet. Thickness varies slightly between suppliers and batches.
That's why a shop builds its own bend tables from test bends on its own machines, and corrects flat patterns to match. Your number and theirs will be close, but theirs is calibrated to what will actually happen at the brake.
What this means for the files you send
If your part has bends, a STEP model of the finished shape is the most useful file. The shop applies its own K-factor or bend deduction and produces the flat blank for cutting. Our post on flat pattern vs 3D model covers when each is the right thing to send.
If you must send a flat DXF, ask the shop for its K-factor or bend deduction for your material and thickness first, and build the flat pattern with that. Mark the bend lines and directions on a separate layer, and state the radius you assumed.
Also remember that the flat length only gets you to the right angle if the brake bends to the right angle. Material springs back after bending, and shops compensate by overbending. Our explainer on springback covers that side.
Getting your part bent
Our CNC bending service builds flat patterns from your 3D model or drawing, so you don't have to know our K-factor. Send the file with material, thickness, bend radius (or "standard"), and quantity. If you've built your own flat pattern, say so in the notes and tell us what K-factor and radius you used.
When you're ready, start a quote for CNC bending.