Bending Guidelines

Use these guidelines to design sheet metal parts that quote cleanly, bend reliably, and avoid surprises during production. The most important checks are bend angle, material thickness, flange length, reverse-bend clearance, and feature placement near bends.

File Checklist

Before uploading a bent sheet metal part, check these items:

1. Export the part as a 3D STEP file
2. Confirm the material and thickness are in our bending range
3. Confirm each bend angle is within our capability range
4. Check minimum flange lengths
5. Check reverse bends, return flanges, channels, joggles, and box shapes for punch clearance
6. Keep critical features outside of the distortion zone

Use the chat bubble or email support@fabworks.com if you have any questions about our process.

Bending Capabilities

Our press brake bends most common sheet metal materials up to 0.250" thick. Following these guidelines gives you the fastest lead time and cleanest parts. If your part falls outside these guidelines, our quoting engine flags it before you order.

Material Range

• Thicknesses: 0.030" to 0.250"
• Materials: Aluminum 5052-H32, Steel 1008, Steel A36, Stainless Steel 304-2B, Galvanized Steel G90
• Maximum bend length: up to 96" depending on material and thickness

For specific thickness and length combinations by material, see the materials pages.

Bend Angle

Available bend angle depends on the material, thickness, and tooling used for the part. Use the material table below to confirm the maximum bend angle for the stock you want to use.

If your part has a return flange, channel, joggle, or boxed shape, also check the reverse bend clearance section. Tooling clearance can limit a part even when the material's bend angle is otherwise allowed.

Bend Radius

Bend radius is set by the tooling used for the selected material and thickness. The material table below lists the bend radius for each stock option.

In most cases, you can use your CAD software's standard sheet metal settings and select the matching material thickness. If you need to hold a tight formed dimension, use the listed bend radius and K-factor values for the exact stock in the table.

Minimum Flange Lengths

The minimum flange length is the minimum length of the straight section of material between the bend and the edge of the sheet. Flanges shorter than this can slip into the V-die or buckle during bending, ruining the part.

Minimum flange length depends on the selected V-die and the bend angle. Material and thickness can change which V-die we use. For the same tooling and angle, sheet thickness does not change the minimum flange length. Use the calculator below to estimate the minimum flange length for your part.

How to Measure Flange Length

Flange length is measured to the apex of the bend, not the length of the resulting flat face. Sharper bends reduce the resulting flat surface area when the flange length stays the same.

Flange Length Calculator

Select the material, thickness, and bend angle. The calculator shows the minimum flange length and an approximate distortion zone. The green dimension shows the minimum flange length. The orange dimension and hatched area show the distortion zone.

Do you want us to check your full part? Upload your STEP file. Our software checks each flange against the minimum length.

Distortion Zone

The distortion zone is the area near a bend where the material stretches and changes shape. Holes and slots in this area can deform. A round hole can become oval. A slot can become angled. An edge can also crack.

Use the minimum flange calculator above to find the approximate distortion zone for your material, thickness, and bend angle. The calculator estimates this zone as 75% of the minimum flange length. Measure the distance from the bend apex, as shown by the orange dimension.

Keep critical holes, slots, and edges outside the distortion zone when their size or position is important.

Is a feature too close to a bend? Upload your STEP file. Our software flags critical features that are inside the distortion zone.

Reverse Bends

A reverse bend is a bend where the punch must enter a channel that was formed by an earlier bend. Examples include a Z-bend, joggle, U-channel, return flange, or box. For these features, punch clearance sets the limit.

Reverse Bend Clearance Checker

Use the beta checker below when your part has a return flange or box feature. The colored curves show the clearance for the punch styles that our quoting engine can select.

Tolerances

• Single bends will be held to a +/- 0.015" length tolerance
• Single bends will be held to a +/- 1 degree angle tolerance
• Features separated by multiple bends will be held to an additional +/- 0.015" for each separating bend
• Die marks will be visible on all bends

K-Factor

The K-factor sets where the neutral axis sits inside a bend, which determines how much your flat pattern stretches when it forms. Get it wrong and your part comes off the brake at the wrong overall dimensions even if the bend angle is correct.

Your CAD software's default K-factor, typically 0.4 to 0.45, is fine for our standard tooling and materials. Don't override it unless you're working to a tight stack-up tolerance, in which case email support@fabworks.com, or use the chat bubble, and we'll give you the exact value to use for your specific material and thickness.

What We Can't Bend

• Single bends longer than 96"
• Bends past the maximum angle listed for that material and thickness
• Reverse bends that exceed the available punch clearance envelope
• Materials not in our standard inventory

Not sure if your part is bendable? Upload your STEP file and our software will check it for you in seconds.

Material Table

Use this table to compare stock thickness, bend radius, minimum flange length at 90°, maximum bend length, and maximum bend angle.