Press Brake forming Basics

Press brake forming is the process of forming sheet metal along a straight axis using punch and die sets.  Typical punch and die combinations include “V” shapes, “U” shapes and in some cases channel shapes.  CNC brake forming is a good fit for small to medium production lots as it eliminates the need for expensive hard tooling. All Humble press brakes can perform “multi-bending” allowing the operator to “step” through complex bend sequences quickly and accurately.

Here are two dimensional views of common brake formed shapes that may be formed on a press brake.  M.T. Offsets will require custom tooling: Forming Basics  Press brake forming-The fundamental advantage of a press brake as a forming tool is its flexibility. By using standard vee-dies, cost savings can be realized through economical set-ups and run times on small lots and prototypes.  In addition to these considerations, using the following guidelines will increase the manufacturability of designs for press brake forming. Dimension the part in a single direction wherever possible. Because of the sequential nature of the forming process, and the fact that dimensional variation is introduced at each bend, dimensioning in a single direction parallels the process and helps to control tolerance accumulation.  Furthermore, allow a more generous bend tolerance (+/- .007”;+/-0.17mm) as tighter tolerances, while achievable, will result in higher costs. Use consistent bend radius for all bends per part, when possible—it helps minimize setup changes. Additionally, we prefer radii specs in fractions of an inch, as our tooling is sized accordingly.  Generally, dimensioning should be done from a feature to an edge. Avoid feature-to-feature dimensions over two or more planes. Feature-to-bend dimensions may require special fixtures or gauging. This also means that tolerances in the title block of a drawing may be unnecessarily restrictive for certain dimensions and angles, while very appropriate for others.   Critical Dimensions Sheet Metal Forming – Outside dimension should be used unless the inside dimension is critical Embosses and Offsets – Emboss and offset dimensions should be to the same side of the material unless the overall height is critical.  .  Bend Radius- As a rule, inside bend radius should be equal to material thickness. When the radius is less than recommended, this can cause material flow problems in soft material and fracturing in hard material. Bend Relief - When a bend is made close to an edge the material may tear unless bend relief is given. Figure "A" shows a torn part. Figure "B" shows a part with the edge a sufficient distance from the form. This distance should never be less than the radius of the bend. Figure "C" shows a bend relief cut into the part, again the depth of the relief should be greater than the radius of the bend. The width of the relief should be a material thickness or greater, preferably a material thickness + 1/64".(0.4mm)

Forming Near Holes – When a bend is made too close to a hole, the hole may become deformed. Figure "A" shows a hole that has become teardrop shaped because of this problem. To save the cost of punching or drilling in a secondary operation the following formulas can be used to calculate the minimum distance required: For a hole < 1" in diameter the minimum distance "D" = 2T + R (see fig. "B") For a slot or hole > 1" diameter then the minimum distance "D" = 2.5T + R (see fig. "C")  

Form height to thickness ratio – To determine the minimum form height for sheet metal use the following formula: D = 2.5T + R (see below) The height can be less but it required secondary operations and is far more costly. 

Edge Distortion – An exaggerated example of edge deformation is pictured in figure "A" below. The overhang caused by this distortion can be as large as ½ the material thickness. As material thickness increases and bend radius decreases the overhang becomes more severe. In situations where an overhang is unacceptable the part can be relieved as in figure "B".