How to Calculate Sheet Metal K-Factor

What Is K-Factor?

When sheet metal bends, the inside surface of the bend is compressed and the outer surface is stretched. Somewhere within the thickness of the metal lies the neutral axis — a line in the material that is neither compressed nor stretched.

The K-factor is the ratio of the neutral axis position to the material thickness:

K = t / T

Where:

• t = distance from the inside surface to the neutral axis
• T = material thickness

A K-factor of 0.5 would mean the neutral axis is exactly in the middle of the material. In practice, bending shifts the neutral axis toward the inside of the bend, so K-factor values typically range from 0.33 to 0.50 depending on the material, tooling, and bending method.

Why Does K-Factor Matter?

If you want a part with a 90-degree bend where one leg measures A and the other measures B, the total flat length is not simply A + B. To get the correct flat pattern, you need to calculate either the Bend Allowance (BA) or Bend Deduction (BD) — and both depend directly on the K-factor.

Get it wrong and:

• Parts won't fit together
• Holes won't line up
• Overall dimensions will be wrong after bending

For a single bend, the error might be 0.5–1mm. But for a part with 4 or 5 bends, errors accumulate and the part can be several millimetres off.

Bend Allowance vs Bend Deduction

These are two different ways to calculate the same thing — the flat pattern length. Understanding both is important because different CAD programs and shops use one or the other.

Bend Allowance (BA)

Bend allowance is the arc length of the neutral axis through the bend — the amount of material consumed by the bend. You add it to the leg lengths:

Lt = A + B + BA

Bend Deduction (BD)

Bend deduction is the amount you subtract from the sum of the outside dimensions:

Lt = A + B - BD

Where Lt is the total flat length, and A and B are the leg lengths measured from the inside of the bend.

The relationship between them uses the Outside Setback (OSSB):

OSSB = tan(A/2) × (T + R)

BD = 2 × OSSB - BA

Where A is the bend angle, T is thickness, and R is the inside bend radius.

The Bend Allowance Formula

BA = π × (R + K × T) × (A / 180)

Where:

• BA = bend allowance
• R = inside bend radius
• K = K-factor (t / T)
• T = material thickness
• t = distance from inside face to neutral axis
• A = bend angle in degrees (the angle through which the material is bent)

This formula works well provided you know the correct K-factor to use. Try our K-Factor Calculator to compute bend allowance, bend deduction, and flat length interactively.

K-Factor Tables by Bending Method

The K-factor depends on the bending method, the ratio of bend radius to material thickness, and the material hardness. The tables below give rule-of-thumb values for the three main bending methods.

Air Bending

Air bending is where the punch touches the workpiece but the workpiece does not bottom out in the lower die cavity. As the punch releases, the workpiece springs back (typically 5–10 degrees). The inner radius equals the punch tip radius. Air bending requires the least force and allows different angles without changing dies — the angle is controlled by punch stroke depth.

Bottoming

Bottoming (or bottom bending) is where the punch and workpiece bottom out on the die. This produces a controlled angle with very little spring-back. The inner radius should be a minimum of 1 material thickness. Bottoming requires about 50–60% more force than air bending but gives more consistent results.

Coining

Coining is where the punch and workpiece bottom on the die and additional compressive stress is applied to the bend zone, increasing plastic deformation. This virtually eliminates spring-back. The inner radius can go down to 0.75 of material thickness. Coining requires the most force.

Key takeaway: Tighter bends (small R/T ratio) shift the neutral axis further toward the inside, giving a lower K-factor. As the radius increases relative to thickness, the K-factor approaches 0.50 regardless of method or material.

Worked Example

Given:

• Material: 3mm mild steel, medium hardness
• Bend radius: 3mm (R/T = 1.0, falls in "T to 3T" range)
• Bend angle: 90°
• Bending method: Air bending
• K-factor from table: 0.43

Bend allowance:

BA = π × (3 + 0.43 × 3) × (90 / 180)

BA = π × (3 + 1.29) × 0.5

BA = π × 4.29 × 0.5

BA = 6.74mm

Outside setback:

OSSB = tan(90/2) × (3 + 3) = 1.0 × 6 = 6.00mm

Bend deduction:

BD = 2 × 6.00 - 6.74 = 5.26mm

If the part has two flanges of 50mm each (measured from the inside of the bend):

Using BA: Flat = 50 + 50 + 6.74 = 106.74mm

Using BD: Flat = 50 + 50 - 5.26 = 94.74mm (note: BD method uses outside dimensions, so with outside dims of 53mm each: 53 + 53 - 5.26 = 100.74mm)

You can verify these calculations with our interactive K-Factor Calculator.

Reverse Engineering the K-Factor

Published tables are a starting point, but every press brake, tooling set, and material batch behaves slightly differently. The most accurate method is to reverse-engineer the K-factor from a physical test bend.

Step-by-Step Method

1. Cut a test strip of known length and thickness. Measure both as accurately as possible. Width doesn't matter much — around 100mm works well.

1. Bend the strip to 90° using the exact same tooling, die opening, and settings you'll use in production. This is critical — whatever you measure now must be reproducible later.

1. Measure the bent piece — record Length X (one leg) and Length Y (other leg), the bend radius, and the bend angle.

1. Calculate using these formulas:

Bend Deduction = Length X + Length Y - Total Flat Length

Outside Setback = tan(Bend Angle / 2) × (Thickness + Bend Radius)

Bend Allowance = (2 × Outside Setback) - Bend Deduction

K-Factor = (-Bend Radius + (Bend Allowance / (π × Bend Angle / 180))) / Thickness

Note on bend radius measurement: The bend radius can be difficult to measure precisely, but small inaccuracies are acceptable. The calculated K-factor will compensate for any measurement error in the radius — it gives you a number that, when used with your CAD program's bend radius setting, will reproduce the real-world result. If the calculated K-factor falls outside 0–1, double-check your measurements.

Use our Reverse Engineer K-Factor calculator to do this calculation automatically.

Bending Tips and Design Guidelines

These practical guidelines apply to all bending methods:

• Consistent bend radii — keep the same radius for all bends in a part to minimise setup changes on the press brake
• Minimum inner radius — should be at least 1× material thickness for most materials
• Grain direction — bending perpendicular to the rolling direction is easier and less prone to cracking. Bending parallel to the grain can cause fracture in hard materials. For cold-rolled steel above Rockwell B 70, avoid bending parallel to the rolling direction
• Minimum flange width — at least 4× material thickness plus the bend radius. Shorter flanges can cause distortion or slippage, risking damage to tooling or the operator
• Holes near bends — holes or slots should be located a minimum of 3× material thickness plus the bend radius from the bend line. If a hole must be closer, extend it past the bend line to prevent distortion
• Dimension stacking — account for tolerance accumulation on multi-bend parts. Make mounting holes oblong where possible to absorb variation

For more design rules, see our complete sheet metal design guide.

K-Factor in CAD Software

Most sheet metal CAD tools let you specify the K-factor (or the related bend allowance / bend deduction) in your sheet metal parameters:

• SolidWorks: Sheet Metal feature → Edit Sheet Metal Parameters → K-Factor
• Fusion 360: Sheet Metal Rules → K Factor
• Inventor: Sheet Metal Defaults → Unfold Rule → K-Factor
• Pro/E (Creo): Uses Y-factor instead, where Y-factor = K-factor × π / 2

Set this correctly and your flat patterns will be accurate from the first cut. If your CAD software asks for Y-factor rather than K-factor, multiply your K-factor by π/2 (approximately 1.5708).

Common Mistakes

1. Using CAD defaults — Many CAD programs default to K-factor 0.44 or 0.50. This may not match your material and tooling. Always verify against your specific setup.

1. Ignoring material condition — Hardened or work-hardened material has a higher K-factor than annealed material. The same alloy can have very different K-factors depending on temper.

1. Not accounting for die width — In air bending, the V-die opening width affects the effective bend radius, which affects the K-factor. A wider V-die produces a larger radius than the punch tip radius.

1. Mixing up BA and BD — Bend allowance is added to inside dimensions. Bend deduction is subtracted from outside dimensions. Make sure you know which one your CAD tool or shop uses.

1. Ignoring grain direction — The same material can behave differently depending on whether you bend with or against the rolling direction. Test both if your parts require bends in multiple directions.

Summary

• K-factor defines where the neutral axis sits during bending (typically 0.33–0.50)
• Use the correct table for your bending method: air bending, bottoming, or coining
• Tighter bends (R < T) have lower K-factors; large radii (R > 3T) approach K = 0.50
• For production work, reverse-engineer K-factor from test bends on your actual equipment
• Set K-factor correctly in your CAD software's sheet metal parameters

Use our free K-Factor Calculator to look up K-factors, calculate bend allowance and bend deduction, compute flat lengths, and reverse-engineer K-factor from physical measurements.

Need parts bent accurately? Our 135-tonne press brake and instant quoting system account for proper bend allowances automatically. Upload your STEP file and get a price in seconds — try our instant sheet metal quoting tool. For more DFM tips on bend radii, flange lengths, and hole placement, see our sheet metal design guide and Laser Cutting Design Guide.