What does K-factor mean in fabrication?

When sheet metal is bent, the outside of the bend stretches and the inside compresses. Somewhere between the two is a layer that does neither: the neutral axis. Its length doesn't change, so it's the line used to work out how long the flat part needs to be.

In flat sheet the neutral axis sits in the middle of the thickness. In a bend it moves towards the inside, and the K-factor records where it ends up:

• K-factor = distance from the inside surface to the neutral axis, divided by the material thickness
• 0.5 means the neutral axis is still in the middle
• 0.33 means it's a third of the way through from the inside

Typical starting values for air bending:

• mild steel: about 0.44
• stainless steel: about 0.45
• soft aluminium such as 5052: about 0.38 to 0.42
• copper and brass: about 0.35 to 0.40

Bottoming and coining push the K-factor higher. Treat all of these as starting points: material, tooling and bend radius all shift the real value.

How is K-factor used?

K-factor is mostly a CAD setting. The sheet metal tools in programs such as SolidWorks, Inventor and Fusion use it to calculate the bend allowance for every bend, then unfold the 3D model into the flat pattern that gets laser cut.

A worked example: an L-bracket in 2 mm (0.08 in) mild steel, 50 mm (about 2 in) on each outside leg, with a 90° bend and a 2 mm inside radius.

• Bend allowance with K = 0.44: 1.571 x (2 + 0.44 x 2) = about 4.52 mm (1.571 is pi/2, for a 90° bend)
• Outside setback: 2 + 2 = 4 mm
• Bend deduction: 2 x 4 - 4.52 = about 3.48 mm
• Flat length: 50 + 50 - 3.48 = about 96.5 mm (3.80 in)

Shops that want accurate flat patterns find their own K-factor with a test bend. They cut a strip to a known length, bend it on the press brake with the tools they'll use, measure the legs, and work back to the K-factor. Doing this for each common material, thickness and die gives a table that matches the shop's brake.

Why does K-factor matter?

K-factor decides whether a bent part comes out the right size. Change it from 0.33 to 0.5 in the example above and the flat length moves by about 0.5 mm (0.02 in). That's one bend. On a part with four bends along one length the error can stack to around 2 mm (0.08 in), enough for a box that won't close or holes that don't line up across a bend.

The usual source of trouble is a mismatch between the K-factor in the designer's CAD and what the shop's press brake actually produces. CAD defaults differ: Inventor ships with 0.44, and SolidWorks is often left at 0.5. If a customer sends a flat DXF unfolded with a generic K-factor, the parts can come out wrong even though the shop cut exactly what it was sent.

K-factor, bend radius and the press brake

In air bending, the inside radius isn't set by the drawing. It comes from the die: roughly 16% of the V-die opening for mild steel, and around 20 to 22% for 304 stainless. A 16 mm (5/8 in) die in mild steel forms an inside radius of about 2.5 mm. If the radius in CAD doesn't match the one the brake forms, the flat pattern is off even with the right K-factor.

That's why shops prefer a 3D model, or a flat pattern built with their own bend data. When a customer sends a flat DXF, it's worth asking what K-factor and inside radius it was unfolded with, or checking one bent dimension on the first part off the brake.

K-factor and quoting

K-factor changes the flat blank by fractions of a millimetre, so it barely moves the material or cutting price. What it changes is risk: a flat pattern built on the wrong K-factor can mean a batch of parts that won't fit, re-cut at the shop's cost. When quoting bent parts, settle who owns the flat pattern before the price goes out.

The folding itself is what moves the price. In Tempus Tools, folding is priced from the longest fold and the number of folds, which set the tool sets, setup time and press time, plus the part's size and weight for handling. When a customer sends a 3D model, Tempus Tools finds the sheet metal parts and unfolds them into flat patterns for quoting.

Further reading: Sheet metal bending: a practical guide for fabrication shops