About Us Machines How It Works Materials Sheet Metal Cutting Blog Contact
DXF & STEP Analysis Sheet Calculator Get a Quote
TR EN
Log In Sign Up

What Is K-Factor? How to Calculate Sheet Metal Flat Patterns for Press Brake Bending

Fabensan Editorial 10 min read

What is the K-factor?

Short answer: The K-factor is the ratio that shows where the layer that keeps its length during bending (the neutral axis) sits within the sheet thickness. It usually falls between 0.30 and 0.50 and is used to calculate the correct length of the flat blank (the flat pattern) that is laser cut before bending.

When sheet metal is bent, the outer surface stretches and the inner surface is compressed and gets shorter. Between these two surfaces there is a layer that neither stretches nor shrinks: the neutral axis. The length of the flat blank equals the length of this layer in the bent part. That is why flat pattern calculations depend on knowing where the neutral axis is.

The K-factor describes that position:

K = t / T

  • t: Distance from the inner surface of the sheet to the neutral axis
  • T: Sheet thickness

If K = 0.50, the neutral axis is exactly in the middle. If K = 0.33, the neutral axis is closer to the inner surface, meaning the inside has been compressed more. In practice the K-factor never goes above 0.50.

If the wrong K-factor is chosen, the part comes out shorter or longer than the drawing after bending. A difference of a few tenths of a millimetre per bend can add up to several millimetres on a part with many bends and cause problems at assembly.

Bend allowance, bend deduction and flat pattern formulas

Three concepts are used in flat pattern calculations. All of them rely on the same K-factor; which one you use depends on how the dimensions are given on the drawing.

1. Bend allowance (BA)

The arc length of the neutral axis through the bend.

BA = (π / 180) × A × (R + K × T)

  • A: Bend angle (degrees; the angle the sheet turns through, 90 for a 90° bend)
  • R: Inside bend radius (mm)
  • K: K-factor
  • T: Sheet thickness (mm)

2. Outside setback (OSSB)

The distance from the start of the bend to the virtual sharp corner where the extensions of the two outer surfaces meet.

OSSB = tan(A / 2) × (R + T)

3. Bend deduction (BD)

The amount to subtract from the sum of the outside dimensions.

BD = 2 × OSSB − BA

Flat pattern length: two routes, same result

  • If the drawing gives outside dimensions: Flat length = Outside dimension 1 + Outside dimension 2 − BD
  • If the drawing gives flat leg lengths (up to the start of the bend): Flat length = Flat leg 1 + Flat leg 2 + BA

For parts with several bends, BD or BA is calculated for each bend and added up.

K-factor chart

The K-factor is not calculated; it is chosen from a chart and, if needed, confirmed with a test bend. Three things decide the choice: the hardness of the material, the bending method, and the ratio of inside radius to sheet thickness (R/T).

Material groups: Soft = materials such as aluminium and copper. Medium = mild steels such as S235, S275 and cold rolled sheet. Hard = stainless steel and high-strength steels.

Air bending (the most common press brake method)

  • Inside radius smaller than thickness (R < T): Soft 0.33 · Medium 0.38 · Hard 0.40
  • Inside radius 1 – 3 times thickness (T ≤ R ≤ 3T): Soft 0.40 · Medium 0.43 · Hard 0.45
  • Inside radius more than 3 times thickness (R > 3T): All materials 0.50

Bottoming

  • R < T: Soft 0.42 · Medium 0.44 · Hard 0.46
  • T ≤ R ≤ 3T: Soft 0.46 · Medium 0.47 · Hard 0.48
  • R > 3T: All materials 0.50

Coining

  • R < T: Soft 0.38 · Medium 0.41 · Hard 0.44
  • T ≤ R ≤ 3T: Soft 0.44 · Medium 0.46 · Hard 0.47
  • R > 3T: All materials 0.50

Practical starting values: For mild steel air bent in a standard V-die (die opening 6 – 8 times the sheet thickness), around 0.44 is common; around 0.45 for stainless steel, and 0.38 – 0.42 for soft aluminium.

Source: Generic K-factor chart, METU Mechanical Engineering "Sheet Metal Work" course notes.

Step-by-step worked example

Example 1: L-bracket

An L-bracket with a 90° bend and outside dimensions of 50 mm × 30 mm is to be made from 2 mm S235 sheet. The inside bend radius is 3 mm and the method is air bending.

  1. Choose the K-factor: R / T = 3 / 2 = 1.5. This ratio is between 1 and 3, and the material is medium (mild steel). From the chart, K = 0.43.
  2. Calculate the bend allowance: BA = (π / 180) × 90 × (3 + 0.43 × 2) = 1.5708 × 3.86 = 6.06 mm
  3. Calculate the outside setback: OSSB = tan(45°) × (3 + 2) = 5.00 mm
  4. Calculate the bend deduction: BD = 2 × 5.00 − 6.06 = 3.94 mm
  5. Find the flat length: 50 + 30 − 3.94 = 76.06 mm

Check with the other route: the flat legs are 50 − 5 = 45 mm and 30 − 5 = 25 mm. 45 + 25 + 6.06 = 76.06 mm. Both methods give the same result.

Example 2: U-channel

With the same sheet and bending conditions, a U-channel with outside dimensions of 40 × 60 × 40 mm is to be made. Because there are two bends, the bend deduction is subtracted twice:

40 + 60 + 40 − 2 × 3.94 = 132.13 mm

If 0.50 had been used by mistake instead of 0.43, the flat blank would come out about 0.2 mm too long per bend. On the U-channel the error is 0.4 mm; on a box with six bends it exceeds 1 mm.

What affects the K-factor?

The K-factor is not a fixed property of the material. The same sheet can give a different K-factor in a different shop or with a different die. The main factors are:

  • Inside radius to thickness ratio (R/T): The most decisive factor. As the radius gets smaller, the inside is compressed more and the K-factor drops. Once the radius exceeds 3 times the thickness, the K-factor approaches 0.50.
  • Material hardness: The K-factor is slightly higher for hard materials (stainless, high-strength steel) and lower for soft materials (aluminium, copper).
  • Bending method: Values are lowest in air bending and higher in bottoming and coining.
  • Die opening (V-die): In air bending the inside radius is set by the die, not the punch. Rule of thumb: the inside radius is about 1/6 of the die opening. A wider die gives a larger radius and a higher K-factor.
  • Grain direction: Bends parallel to the rolling direction carry a higher risk of cracking and can change the result. On critical parts, keep the bend line perpendicular to the rolling direction.
  • Material batch: Even sheets of the same grade can differ in thickness and yield strength. In series production, measuring the first part and confirming the K-factor is the safest approach.

How to find the K-factor with a test bend: Cut a strip of known length and bend it to 90°. Measure the two outside dimensions and the inside radius. Work out the bend allowance from the measurements and reverse the formula: K = (BA × 180 / (π × A) − R) / T. This value is your real K-factor for that machine, die and material.

K-factor in CAD software and common mistakes

When designing sheet metal parts in programs such as SolidWorks, Fusion 360, Inventor and Onshape, the K-factor is entered in the material or sheet metal settings. The program calculates the flat pattern with this value, and that is where you export the DXF for laser cutting.

Common mistakes:

  • Leaving the default value: Many programs use a single default value such as 0.50 or 0.44. For tight-radius bends this makes the flat pattern too long.
  • Using the same K-factor for every thickness: 1 mm and 10 mm sheet cannot be bent with the same die; the R/T ratio changes, and so does the K-factor.
  • Drawing an inside radius that cannot be produced: Specifying a 1 mm inside radius on a 10 mm sheet means that radius will not form in the shop. Choose the inside radius to match the manufacturer's tooling.
  • Mixing up bend deduction and bend allowance: If you work with outside dimensions, subtract BD; if you work with flat leg lengths, add BA. Mixing the two doubles the error.
  • Calculating without a material certificate: For stainless or high-strength steel, check the yield strength on the certificate; a harder batch changes springback and the K-factor.

The safest approach: For critical parts, send your drawing to the manufacturer with the inside radius and bend angle, and let them prepare the flat pattern with the machine's real K-factor.

Frequently asked questions

What should the K-factor be?

There is no single correct value. For air bent mild steel with an inside radius of 1 – 3 times the thickness, 0.43 – 0.44 is a good starting point. Around 0.45 is used for stainless and 0.38 – 0.42 for soft aluminium.

Why can't the K-factor be greater than 0.50?

In bending, the inner surface is compressed and the outer surface stretches. The neutral axis therefore either stays in the middle or shifts towards the inner surface; it does not move towards the outer surface.

What is the difference between bend allowance and bend deduction?

Bend allowance is the arc length added to the flat leg lengths. Bend deduction is the amount subtracted from the sum of the outside dimensions. Both give the same flat pattern; only the starting dimensions differ.

Does the formula change for angles other than 90 degrees?

No. The A in the formulas is the angle the sheet turns through. For example, for a bend with an included angle of 120°, the sheet turns 60°, so A = 60.

Where do I enter the K-factor in CAD?

There is a "K-Factor" field in the sheet metal properties or the material definition. If you use a bend table, the values in that table apply instead of the K-factor.

Should I prepare the flat pattern or should the manufacturer?

For simple parts you can prepare it yourself using chart values. For tight tolerances or parts with many bends, it is safer to send the 3D model (STEP) and have the flat pattern prepared with the manufacturer's machine data.

Order bent parts without the flat pattern maths

At Fabensan, laser cutting and press brake bending are done under one roof. If you send your 3D model (STEP), we prepare the flat pattern with the real K-factor of our own machines and tooling. If you send a DXF, we check your flat pattern before bending. Our press brakes handle parts up to 12 metres long.

There is no minimum order; we quote anything from a single prototype to series production.

  1. Sign up at fabensan.com and upload your STEP, DXF, DWG or PDF drawing.
  2. Enter the material, thickness and quantity. If you are unsure about the inside radius or tolerances, mention it in the notes.
  3. Get your quote and approve it; your parts are delivered cut and bent to your door.

Before uploading, you can run a quick check with the DXF & STEP Analysis tool on our website.