Get an instant quote
Get in touch Listen to our podcast
design tips to help reduce overall cost of sheet metal parts

How to Design Features for Sheet Metal Bending - Complete Design Guide

Rapid prototyping
and full-scale production
ISO accredited
& QC checks
All in-house
processes
Used in over
50 countries
FREE Instant
quotations

Bending is a fundamental process in sheet metal working that involves deforming a metal workpiece into a desired shape by applying force between two tools by a press brake: an upper tool (known as a punch) and a bottom tool (known as a V-die). Bending can improve a part’s structural integrity by increasing part stiffness, redistributing stress within a part, and help achieve specific shapes that are required for certain applications. For instance, shaping a curved profile can improve a part’s ability to withstand certain types of loads.

 

Sheet metal bending process and design guide

 

To fully utilize the capabilities of this process, it is important that your CAD is designed according to a number of recommendations. In this article, we offer a comprehensive guide to the best design practices for Sheet Metal Bending, tolerance guide and cost reduction tips.

 

Sheet metal bending: designing guidelines

 

Rules for Designing Bends

The basic bending design guidelines that a designer needs to consider when modelling a sheet metal component include wall thickness, bend radii, and bend allowance.

 

 

1. Wall thickness

Sheet metal parts are usually fabricated from a single sheet of metal, so they should have a uniform wall thickness. Generally capabilities of of 0.9mm – 20mm in thickness are able to be manufactured from sheet (<3mm) or plate (>3mm) but this tolerance depends mainly on the part.

 

2. Bend radii

At a minimum, the smallest bend radius should be at least equal to the sheet thickness to avoid fractures or distortions in the metal part. Keeping bends in the same plane in the same direction helps to save time and money by preventing part reorientation. Keeping the bend radius consistent will also make parts more cost-effective.

 

3. Bend allowance

When you bend sheet metal, the neutral axis shifts toward the inside surface of the bend. The ‘K-factor’ is the ratio of the neutral axis location (t) to the material thickness (T), which can be used to to calculate the bend allowance. View the K-factor chart below to calculate the amount of material needed to account for your bend.

 

K-factor chart
RadiusAluminium (Soft)Aluminium (Medium)Stainless Steel (Hard)
Air bending
0 – t0.330.380.40
t. – 3*t0.400.430.45
3*t. – >3*t.0.50
0.50
0.50
Bottom bending
0 – t.
0.42
0.44
0.46
t. – 3*t.0.46
0.47
0.48
3*t. – >3*t.0.50
0.50
0.50
Coin bending
0 – t.
0.38
0.41
0.44
t. – 3*t.0.44
0.46
0.47
3*t. – >3*t.0.50
0.50
0.50

 

 

Rules for Designing Bend Relief

Bend reliefs are two small cuts made in a piece of sheet metal to free up the metal between them. Although they are small features, leaving them out can cause stress to concentrate at the bend line, resulting in deformed holes and slots.

 

1. Bends close to an edge

If bend reliefs are left out for bends made close to an edge, it can cause unwanted tearing. In some cases, it can make your part un-manufacturable. To ensure successful bending, the width of the relief cuts should be at least equal to the material thickness, and the length should be longer than the radius of the bend.

 

adding bend relief design for sheet metal parts

 

2. Bends where the flanges aren’t adjoining

Flange in sheet metal parts, is a feature that consists of a face and bend connected to an existing face along a straight edge. For bends where the flanges aren’t adjoining, there are a number of different relief types available for utilisation by designers. Two of the most common types include:

 

  • Oblong Relief: They have rounded ends, which help in distributing the stress more evenly compared to sharp corners. Oblong reliefs are particularly useful useful when the bend is close to holes or slots, as they minimise the distortion of these features by allowing more controlled movement of the material.
  • Rectangular Relief: Rectangular reliefs are straightforward to cut and require less complex and costly tooling, suitable for designs where the bend radius is not too tight, and the material thickness is within a manageable range.

 

designing rectangular and oblong relief in sheet metal parts

 

Rules for Designing Edge Features

Some components benefit from having special features formed from the remaining edges, two of these main features are curls and hems.

 

1. Curl edge guidelines

Curls are hollow circular rolls formed at the edge of the sheet via sheet metal bending. Curl features are commonly used to provide strength to a part and to remove sharp edges from the workpiece so that it is safe to handle.

 

Example of curl edge feature on sheet metal part

 

For best results, it is recommended that the outer radius of a curl be at least twice the material thickness, although this will vary depending on the manufacturer and their tooling for curling. The bend should be at least the radius of the curl plus 6 times the material thickness from the curl feature

 

2. Hem edge guidelines

Hems are similar to curls — they are folds made back onto the metal itself — formed into a U shape. Hem features are commonly used to provide strength to the part and connect parts together. The three main types of hem features industrial and designers should be familiar with include: open hem, closed hem, and teardrop hem.

 

top 3 hem types in sheet metal bending

 

  • Open Hem: This type of hem has a slight gap or space, leaving the fold partially open. The minimum recommended inside diameter equals the material thickness and a return length of 4 times the thickness is recommended.
  • Closed Hem: This type of hem is tightly closed with no gap. It is recommended that the minimum inside diameter equals the material thickness, and the hem return length is 6 times the material thickness.
  • Teardrop Hem: This type of hem forms a teardrop shape, providing a compromise between strength and material flexibility. The minimum inside diameter should be at least equal the material thickness, and a return length of 4 times the thickness is recommended.

 

Open hems used to connect two sheet metal parts

Example of how open hems can be used to connect two parts

 

Rules for Designing Hole Features

 

1. Holes and slots positioned too close to bends

Holes and slots which are located close to bends are susceptible to deforming following bending. To ensure successful bending, it is recommended to place holes away from bends at a distance of at least 2.5 times the material’s thickness (T) plus the bend radius (R). For slots, it is recommended to position it at least 4 times the material’s thickness plus the bend radius away from the bend.

 

  • Minimum recommended hole edge from bend face = 2.5T + R
  • Minimum recommended slot edge from bend face = 4T + R

 

Sheet metal hole and slot design

 

2. Holes and slots positioned too close to edge

Holes and slots located too near a part edge can result in a ‘bulging’ effect. Therefore, a good rule of thumb is to leave a minimum space of at least 2 times the thickness of the sheet between the extruded holes and the part edge.

 

sheet metal bending techniques and solutions

 

Source custom sheet metal parts

Get a quote with HLH Rapid 24 to 48 hours or less

 

Sheet metal bending tolerance guide

Standard sheet metal bending tolerances for reference:

FeatureTolerance
Forming or bending±0.508mm (0.020″)
Bend to hole or feature±0.254 mm (0.010″)
Bend to hole±0.381 mm (0.015″)
Bend to hardware±0.381 mm (0.015″)
Bend to edge±0.254 mm (0.010″)
Bend to bend±0.381 mm (0.015″)

Sheet metal fabrication services, custom-cut for your project

Source custom sheet metal prototypes and production parts with us from a wide range of metals, including sheet metal alloy, steel and stainless steel alloys, and copper alloys. Simply submit your 2D and 3D CAD drawings to our site contact form along with any project details including quantity, material or surface finishing requirements, and our engineering team will get back with a quote within 24 hours.

Home Banner

Put your parts in production today

Get an instant quote