How to Calculate Bend Deductions for Sheet Metal in SolidWorks

Why Bend Deduction Matters

When a sheet metal press brake bends a flat blank, metal on the inside of the bend is compressed and metal on the outside is stretched. The result: the final bent part has a different total length than the sum of its straight leg lengths. That difference is the bend deduction — and if you don't account for it, your flat pattern will cut to the wrong size.

A classic failure mode: a designer creates a U-channel in SolidWorks, ignores the default K-factor, sends the DXF to the laser cutter, and the fabricated channel comes back 3–4 mm too wide because the flat pattern was calculated with incorrect bend parameters. The tooling is fine. The laser is fine. The problem was always in the design file.

Understanding bend deductions is especially important when you're sourcing from an external fabricator like FYORD, because once your DXF is cut, there's no going back. The laser doesn't know you meant something different — it cuts what it's given.

The Three Core Concepts

Before diving into formulas, let's define the three terms you'll encounter constantly in sheet metal design:

1. Neutral Axis

Every bent sheet has an imaginary line running through it where the material experiences neither compression nor tension — this is the neutral axis. In thin, soft materials bent over large radii, this axis sits almost exactly at the centre of the material. In thick or hard materials bent tightly, it shifts closer to the inside of the bend. The position of this neutral axis determines the K-factor.

2. Bend Allowance (BA)

Bend allowance is the actual arc length of the neutral axis through the bend zone. It's the length of material "used up" in the bend — the portion that is neither part of the first leg nor the second leg, but is curved. To find the correct flat blank size, you take the sum of all straight legs and add the bend allowance for each bend.

3. Bend Deduction (BD)

Bend deduction works from the outside. If you measured the two legs by extending them to where they intersect (their theoretical sharp corner), you'd get a number larger than the real bent part. Bend deduction is the amount you subtract from that theoretical outside measurement. This is what SolidWorks uses in its sheet metal environment by default, and what most press brake operators quote to you.

K-Factor: What It Is and How to Choose It

The K-factor is a dimensionless ratio that describes where the neutral axis sits within the material thickness. It ranges from 0 (neutral axis at the inside face) to 0.5 (neutral axis at the centre) to 1 (neutral axis at the outside face). In practice, almost all sheet metal K-factors fall between 0.3 and 0.5.

Choosing the right K-factor is part engineering, part experience. The variables that affect it are material type (ductility), material thickness, bend radius, and tooling geometry. Here are the commonly used values:

How Bend Radius Affects K-Factor

As a rule: the tighter the bend radius relative to material thickness, the lower the K-factor. A bend radius equal to the material thickness (R = T, sometimes written R/T = 1) pulls the neutral axis inward significantly — use K = 0.33 for this case. For generous radii (R/T > 3), the neutral axis barely moves and K approaches 0.5.

Bend Allowance Formula Explained

Once you have your K-factor, calculating bend allowance is straightforward. The formula calculates the arc length at the neutral axis through the bend angle:

This formula is derived from basic arc geometry: arc length = radius × angle (in radians). The (R + K × T) term is the radius of the neutral axis — the inside radius plus the distance from inside face to neutral axis. Multiplying by π/180 converts the bend angle from degrees to radians.

Flat Pattern Calculation from Bend Allowance

Once you have BA for each bend, the total flat blank length is simply:

Bend Deduction Formula

SolidWorks Sheet Metal works with bend deduction by default. The relationship between bend allowance and bend deduction is:

The term 2 × (R + T) × tan(A/2) is called the "setback" — it's twice the distance from the bend tangent line to the virtual sharp corner. Subtracting the bend allowance from twice the setback gives you the bend deduction.

For flat pattern from bend deduction:

Worked Example: 90-Degree Bend in 2mm Mild Steel

Let's walk through a complete calculation. We have a simple L-bracket in 2mm mild steel (cold-rolled, medium hardness). One leg is 50mm, the other is 30mm, and the press brake tooling has an inside radius of 2mm. Bend angle is 90 degrees.

Setting Up Sheet Metal in SolidWorks

SolidWorks has a dedicated Sheet Metal environment that automates flat pattern creation — but only if you configure it correctly from the start. Here's the recommended setup process.

Starting a New Sheet Metal Part

Open a new part, go to Insert → Sheet Metal → Base Flange/Tab. SolidWorks will ask for:

• Thickness — your material gauge (e.g., 2mm)
• Default Bend Radius — match your fabricator's tooling (typically T to 1.5T for mild steel)
• Bend Allowance / Bend Deduction — where you enter your K-factor or BD value
• Auto Relief — choose "Rectangular" for most sheet metal; set width to at least T and depth to 0.5T

Setting K-Factor in SolidWorks

In the Sheet Metal Feature Manager, under Bend Allowance, select "K-Factor" from the dropdown. Type your K-factor value (e.g., 0.42). This will be used for all bends in the part unless overridden individually. You can also select "Bend Table" or "Bend Allowance" if you want to manually specify values.

Flat Pattern View

Once your part is modelled, right-click the part in the tree and select Flatten, or use Insert → Sheet Metal → Flatten. This unfolds all bends and shows the flat blank with bend lines marked. You can then right-click the flat pattern → Export to DXF/DWG to generate the cutting file.

SolidWorks Gauge Tables and Bend Tables

For production work, manually entering K-factors is error-prone. SolidWorks supports gauge tables — Excel files (.xls) that store thickness, bend radius, and K-factor or bend allowance for each material. When you use a gauge table, changing the material dropdown automatically updates all bend parameters.

Where to Find Gauge Tables

SolidWorks ships with sample gauge tables at: C:\Program Files\SOLIDWORKS Corp\SOLIDWORKS\lang\english\Sheet Metal Gauge Tables\

These samples cover mild steel and aluminium in standard gauges. You can copy and modify them. The Excel format is straightforward: one tab per material, rows are gauge/thickness, columns are bend radius, and cells contain K-factor or bend allowance in mm.

Creating a Custom Gauge Table

To create your own gauge table for, say, 304 stainless:

1. Open one of the sample .xls gauge table files
2. Save As with a new name (e.g., "Stainless_304_Gauge_Table.xls")
3. Update the thickness column to match your stock sizes
4. Update K-factor or BA values using your fabricator's empirical data
5. In SolidWorks Sheet Metal properties, browse to your custom table

If you're ordering from FYORD regularly, ask us for our recommended bend parameters — we can share the empirically-measured values from our press brake for each material and gauge combination we stock.

Bend Tables vs. K-Factor vs. Bend Allowance

Common Mistakes That Ruin Flat Patterns

1. Using SolidWorks Default K = 0.5

The SolidWorks default K-factor is 0.5 — meaning it assumes the neutral axis is exactly in the middle of the sheet. This is theoretically correct for elastic bending of a homogeneous beam but is not accurate for real press brake bending. Most real-world bends have K-factors between 0.38 and 0.46. Using 0.5 will consistently produce flat patterns that are too short.

2. Ignoring Grain Direction

Sheet metal has a rolling direction, and bending across the grain (perpendicular to rolling direction) requires less force and achieves tighter radii than bending with the grain. For aluminium 5052, a bend radius you can achieve across the grain may crack if applied with the grain. DXF files should include a grain direction note if it matters for your part.

3. Not Accounting for Springback

When you remove a bent part from the press brake, it springs back slightly — especially in high-yield materials like stainless and 6061-T6. Springback is not captured in bend deduction calculations; it's a tooling compensation that your fabricator handles by overbending. Inform your fabricator of critical angle tolerances (±1° or better) so they know to compensate.

4. Using Outside Dimensions for Legs in SolidWorks Sketches

When sketching sheet metal flanges in SolidWorks, dimension to the inside face, not the outside. SolidWorks sheet metal features measure flange length from the bend tangent line, not from the outside face. Dimensioning to the outside will cause your legs to be off by one material thickness.

5. Applying the Wrong Bend Radius for the Material

A 1mm inside radius on 3mm aluminium 6061-T6 will crack on the first bend. Always check the minimum bend radius for your material and thickness before modelling. As a rule of thumb: minimum bend radius for 6061-T6 is approximately 3× thickness; for mild steel it's about 1× thickness; for 5052-H32 aluminium it's about 1.5× thickness.

Quick-Reference Table for Common Materials

These values are our recommended starting points for FYORD press brake tooling. They are empirically derived and will give you accurate flat patterns for most standard parts. Tight-tolerance work (<±0.3mm) should always be validated with a physical test bend.

Calculating BA and BD Yourself

Using the formulas above, here's how the 2mm mild steel row was derived:

• BA = (π/180) × 90 × (2 + 0.44 × 2) = 1.5708 × 2.88 = 4.52mm
• BD = 2 × (2 + 2) × tan(45°) − 4.52 = 8 − 4.52 = 3.48mm

You can verify every row in the table using the same arithmetic. Bookmark this page or print the table and tape it to your workstation.

Minimum Bend Radii by Material