Bending is a kind of stamping process that forces materials to generate plastic deformation by using pressure so as to form a certain angle and curvature shape.

The common bending methods include V bending, Z bending and reverse bending.

Contents

- 1 1. Bending height
- 2 2. Bending radius
- 3 3. Bending direction
- 4 4. Avoid bending failure due to impossible materials pressing at bending base
- 5 5. Ensuring proper bend gap to avoid bending interference
- 6 6. Ensuring bending strength
- 7 7. Reducing bending procedures
- 8 8. Avoiding complicated bending
- 9 9. The holes in multiple bending are difficult to align

## 1. Bending height

The bending height of metal plate is at least twice the thickness of the metal plate plus the bending radius, namely H>2t+R.

If the bending height of metal plate is too low, distortion is prone to occur, which makes it difficult to get ideal shape and size.

When bending for bevel edge, bending distortion is easy to occur as the bending height is too small.

As shown in the figure, in the original design, because the left bending height is too small, bending deformation is easy to happen, which causes low bending quality; when trying to optimize the original design, left bending height should be increased or smaller parts requiring small bending should be removed. In this way, distortion will not happen and the bending quality will be high.

## 2. Bending radius

To guarantee bending strength, the bending radius should be larger than material’s minimum bending radius, just like the graph below shows:

Materials Condition | ||
---|---|---|

Materials | Soft | Hard |

Aluminum alloy | 0 | 6t |

Beryllium bronze | 0 | 4t |

Brass | 0 | 2t |

Magnesium alloy | 5t | 13t |

Stainless steel | 0.5t | 6t |

Mild steel, low alloy steel | 0.5t | 4t |

Titanium | 0.7t | 3t |

Titanium alloy | 2.6t | 4t |

The original and improved bending radius of the metal plate is shown in the graph:

It is not to say that the larger the bending radius the better.

The larger the radius is, the larger the bending bounce is, the more difficult the bending angle and bending height to be controlled, so the bending radius of the metal plate should be reasonable.

Metal plate mold manufacturers tend to have a zero bending radius so that it is not easy to rebound and the bending height and bending angle are easy to control.

But such bending is easy to cause an external crack or even broken, at the same time, bending strength of metal plate is relatively low, especially for hard ones.

Besides, after using for a certain time, the right-angle of mold would gradually be smooth, which makes the bending size difficult to control

In order to reduce the bending force and ensure bending size, metal plate mold manufacturers adopt another method, which is to add the line pressing process before the bending, of course, such a design can cause the bending strength is relatively low and easy to crack or break.

The line pressing process is to extrude partial materials to form a groove on the metal plate, which can facilitate the bending and ensure the bending precision.

## 3. Bending direction

When bending, it should be perpendicular to the fiber direction of the metal material.

When the bending is parallel to the direction of the metal material, it is easy to crack at the bending section, so the bending strength is low and easy to break.

## 4. Avoid bending failure due to impossible materials pressing at bending base

When bending metal plate, it is often impossible to press material because other features are too close to the bending base, resulting in the failure of bending or bending deformation.

Generally speaking, there should have no press materials that will affect sheet metal bending at the position on top of the bending base (at least twice the sheet thickness plus bending radius distance).

In the original design, as shown in the figure above, the reverse flatten position is too close to the bending base of the metal plate, causing the bending failure because of impossible material pressing.

As shown in the figure below, in the original design, the extrusion part of the metal plate is too close to bending the base, making the bending infeasible.

Under this situation, the extrusion part should be moved far away from the base position of metal plate; if limited by the design requirements, both the extrusion part and the bending position cannot be moved, then a kerf at the bending base corresponding to the extrusion part should be added, so as to ensure the bending to be carried out smoothly.

## 5. Ensuring proper bend gap to avoid bending interference

Due to the existence of bending tolerance of metal plate, it is necessary to guarantee a certain bending gap in the direction of bending, so as to avoid the failure of bending caused by interference in bending.

As shown in the figure, the bending sequence of parts is:

*first, bend the upper side, then the right side. *

In the original design, the two bending have no gap, then when the upper side bending and right side bending are done, because of the bending tolerance, interference is likely to be caused between the right side bending and the upper side bending.

In the improved design, at least 0.2 mm gap is saved between the right side and the upper side which will effectively avoid the interference.

## 6. Ensuring bending strength

Bending strength should be ensured in metal plate bending.

Long and narrow plates have low bending strength, while the short and wide ones have high bending strength.

So, the bending should adhere to the longer side as much as possible, as shown in the figure.

For the bending with the same function, in the original design, the bending strength is low because the bending adheres to the shorter side, but in the optimized design, the bending strength is high because the bending adheres to the longer side.

## 7. Reducing bending procedures

The more the bending process of the metal plate is, the higher the mold cost, the lower the bending precision.

So in metal plate design, the bending process should be as simple as possible.

As shown in the figure, the original design needs two bending processes while in an optimized design of improvement, only one bending process can realize two bending.

## 8. Avoiding complicated bending

The more complex sheet metal bending process, the higher the mold cost, the lower the precision of bending.

Moreover, the complex bending may result in a waste of parts and materials.

Therefore, when metal plate bending is complex, you can consider splitting it into two parts, and then assembled by the pop rivet, self-clinching or spot welding.

## 9. The holes in multiple bending are difficult to align

Metal plate bending tolerance is relatively large, especially under multiple bending.

Feature | Allowance (mm) |
---|---|

1 bend | 0.15 |

2 bend | 0.25 |

3 bend | 0.36 |

4 bend | 0.44 |

5 bend | 0.51 |

6 bend | 0.59 |

The accumulation of tolerances causes holes is difficult to align.

The more the metal plate bends, the greater the bending tolerance.

The multiple bending is difficult to ensure the accuracy of the bending size, this is why the screw holes, rivet holes, self-clinching holes in metal plate bending are very difficult to align.

**Solution:**

- Design one of the bending hole to be a large hole or a long circular hole, which allows a larger tolerance.
- Add two internal positioning holes, reduce the tolerance of metal plate bending to ensure the alignment of bending holes.
- The size precision of the two holes can be guaranteed by first bending and then drilling, but this will increase the complexity of the stamping die, increase the cost of the mold, and generally is not recommended.

ShadyDecember 16, 2018 at 11:25 amAmazing post. Thanks for sharing information.

MachineMfgDecember 16, 2018 at 10:16 pmGlad to hear that. And we will continue to share amazing post : )