Every flat pattern depends on one number nobody can see: how far the neutral axis sits from the inside surface of the bend, expressed as a fraction of the sheet thickness. That is the K-factor. Put it in a CAD library once and forget it, and every tight radius or new material becomes a part that comes out short.
What is the K-factor in sheet metal?
The K-factor is the position of the neutral axis inside the material during bending, expressed as a fraction of the sheet thickness: K = t / T, where t is the distance from the inside bend surface to the neutral axis and T is the material thickness. In the bend allowance formula BA = π (R + K×T) × A / 180 it is the only input that cannot be measured from the drawing, which is why it is the usual source of a flat pattern that is a few tenths of a millimetre wrong. Typical values run from about 0.33 for a tight bend in a work-hardening material to 0.50 for a generous radius in soft material, and the correct value has to be confirmed on the first article because it moves with the R/T ratio, the material and the tooling.
The rules of thumb, and why they are only a starting point
| Condition | Typical K-factor | What drives it |
|---|---|---|
| Tight bend, R/T below about 1 | 0.33 - 0.40 | The neutral axis sits well inside; the outside stretches hard |
| General bending, R/T around 1-3 | 0.40 - 0.45 | The common workshop range and the usual CAD default |
| Generous radius, R/T above 3 | 0.45 - 0.50 | The neutral axis moves toward the middle of the sheet |
| Work-hardening material (304, 430) | Lower end of the range | Stainless resists flow into the bend differently from mild steel |
| Soft material (aluminium, copper) | Upper end of the range | More deformation before the outer fibre work-hardens |
These are starting values for a calculation, not a specification. Two shops bending the same 1.5 mm DC04 with the same punch and die can legitimately arrive at slightly different values, because the inside radius that actually forms depends on the die opening and on whether the operation is air bending, bottoming or coining.
Why the K-factor is not a constant
- R/T ratio - the single biggest influence. A tight bend in 1 mm sheet and a generous bend in 3 mm sheet are not the same material behaviour even in the same grade.
- Material and temper - the more a material work-hardens, the further the neutral axis shifts toward the inside during the bend.
- Tooling and method - the die opening sets the inside radius in air bending, so a drawing that prints R2 may form at R1.8 or R2.4 depending on the tool that runs it.
- Bend direction against the rolling direction - small, but real on a part with several bends, and it explains a flat pattern that fits in one orientation and not the other.
- Springback correction - a press brake that compensates for springback changes the effective bend geometry, and with it the value that should be in the calculation.
How we set it in production
We start from the drawing, calculate the flat length with a K-factor in the usual range for that material and R/T, cut and form the first part, measure the finished legs, and correct the value before the batch runs. For a single-bend bracket that is a two-minute loop. For a welded frame with a dozen bends it is what stops the frame arriving at the welding table two millimetres out over its length. Where the part is formed in a die rather than on a brake, the geometry comes from the tool and the flat pattern from the strip layout, so the two routes carry different numbers and are never mixed.
What to send if you want a flat pattern
- The finished part drawing, with every bend angle and inside radius stated.
- Material and thickness, with the temper or condition if it is not the standard one.
- Whether the part will be air bent, bottomed or coined, if that is already decided.
- The dimensions that must be held: overall outside size, hole-to-bend distance, or the flat blank itself.
- Any bend that runs across the rolling direction, if the visible grain matters.
Key point
K-factor is an input to the bend allowance, not a property of the material, and it is only correct for the R/T, material and tooling it was measured on. Confirm it on the first article and keep it with the part record - after that the flat pattern is repeatable for the life of the programme.
Frequently asked questions
What is a typical K-factor for sheet metal?
Between 0.33 and 0.50. A tight bend in a work-hardening material sits near 0.33, a generous radius in soft material near 0.50, and most general bending sits at about 0.40-0.45.
Is K-factor the same as the Y-factor?
No, but they are related. The Y-factor scales the K-factor to account for springback and material behaviour: Y = K × π/2, so the two are used in different versions of the same bend allowance calculation.
Why is my flat pattern wrong even though I used the standard K-factor?
Because the inside radius that actually forms is set by the die opening and the method (air bending, bottoming, coining), not by the radius printed on the drawing. Confirm the finished legs on the first part and correct the K-factor.
Can you give me the flat pattern for a part I designed?
Yes. Send the finished drawing with bend angles and inside radii, the material and thickness, and the dimensions that must be held, and we will return the flat length we will actually cut.