Home/Tools/K-Factor Calculator
Free engineering tool

Sheet Metal K-Factor Calculator

Find the K-factor from a test bend, or enter a K-factor to get the bend allowance, bend deduction and flat length of a bent part. Or pick a material, thickness and tooling to get the 90° bend deduction Komacut measured for that setup.

✓
Works both ways
Find K from a test bend, a bend allowance or a bend deduction. Or start from K.
✓
Every layout value
Bend allowance, bend deduction, outside and inside setback, neutral axis and Y-factor.
✓
Komacut measured data
90° bend deductions for Komacut materials, by thickness, punch and die.
How it works

How to use the K-factor calculator

Switch between mm and inches at any point. Bend deduction by material uses values Komacut measured in its China facility, for 90° bends.

01

Pick what you know

Find the K-factor if you have a test bend, a bend allowance or a bend deduction. Use a K-factor if you already have one and need the flat length. Bend deduction by material gives the measured 90° bend deduction for a Komacut material.

02

Enter the bend

Thickness, inside radius and bend angle. The bend angle is the angle the flange turns through: 90° for an L-bracket. If your drawing gives the included angle, enter 180° minus that angle. For bend deduction by material, pick the material, thickness, punch radius and die opening instead.

03

Read the results

Depending on the mode, the main result is the K-factor, the flat length or the bend deduction. The other bend values are listed below it.

Definition

What is the K-factor in sheet metal?

The K-factor is the distance from the inside face of the bend to the neutral axis, divided by the material thickness: K = t ÷ T. Published values are typically between 0.3 and 0.5.

When sheet metal bends, the inside of the bend is compressed and the outside is stretched. The neutral axis is the layer between them that keeps its original length. Because its length does not change, the arc it follows through the bend is the bend allowance: the length of flat material the bend uses.

The neutral axis moves toward the inside of the bend as it forms, so K is below 0.5 in most bends. How far it moves depends on the material, the ratio of inside radius to thickness (R/T), the bending method and tooling, and the rolling direction of the sheet.

Quick reference
K-factor in three lines
K-factorK = t ÷ T
Typical range0.3 to 0.5
Y-factorY = K × π / 2
Formulas

K-factor, bend allowance and bend deduction formulas

Bend allowance
BA = π/180 × A × (R + K × T)
K-factor
K = (180 × BA ÷ (π × A) − R) ÷ T
Outside setback
OSSB = tan(A/2) × (R + T)
Bend deduction
BD = 2 × OSSB − BA
Flat length, outside flanges
L = L1 + L2 − BD
Flat length, inside flanges
L = L1 + L2 − 2 × R × tan(A/2) + BA

A is the bend angle in degrees, R the inside radius and T the thickness. L1 and L2 are the flange lengths measured to the apex, where the extended outer (or inner) faces of the two flanges meet. For parts with several bends, subtract one bend deduction per bend.

Worked example
2 mm sheet, R 2 mm, 90° bend, K 0.38
Bend allowanceπ/180 × 90 × (2 + 0.38 × 2) = 4.335 mm
Outside setbacktan 45° × (2 + 2) = 4.000 mm
Bend deduction2 × 4.000 − 4.335 = 3.665 mm
Flanges (outside)50 + 50 mm
Flat length100 − 3.665 = 96.335 mm
FAQ

Frequently asked questions

What is a typical K-factor?

Most published values are between 0.3 and 0.5. The exact value depends on the material, the ratio of inside radius to thickness, the bending method and the tooling.

How do you calculate the K-factor?

Bend a test strip, measure the flat length and both flanges, and work out the bend allowance. Then K = (180 × BA ÷ (π × A) − R) ÷ T. The calculator does this under Find the K-factor.

Why does the bend deduction change with the die?

In air bending, the V-die opening mainly sets the inside radius. A wider die gives a larger radius and, in most cases, a larger bend deduction. In Komacut's data, 2.0 mm SPCC with an R1 punch has a bend deduction of 3.51 mm on a V12 die and 3.80 mm on a V16 die.

What is the difference between bend allowance and bend deduction?

Bend allowance is the length of the neutral axis through the bend. Bend deduction is what you subtract from the outside flange lengths to get the flat length. They are linked: BD = 2 × outside setback − BA.

What is the Y-factor?

Another way to state where the neutral axis sits, used by some CAD software such as Creo. Y = K × π/2, so K = 0.33 equals Y = 0.52.

Do I enter the bend angle or the included angle?

The bend angle: the angle the flange turns through from flat. Bend angle = 180° − included angle. A 90° L-bracket has both at 90°. A flange with a 60° included angle has a 120° bend angle.

Know the flat length? Get the part price.

Upload your STEP, STP or SLDPRT file to Komacut and get a quote in about 30 seconds, with a design check and volume pricing from 1 piece to thousands. No minimum order.

Get an instant quote →

Free account · No MOQ · STEP / STP / SLDPRT