How to design precision sheet metal components for laser cutting, cnc punching and folding.
The aim of this guide is to provide designers with simple hints and tips to allow them to design sheet metal components that are easy to manufacture, and therefore cost effective, whilst maintaining maximum precision and quality.
Before reading this guide it is recommended that you take a look at How Sheet Metal Bending Works to fully understand how the pressbrake machine operates and the different types of tooling. The majority of folded parts at Hydram are formed using air bending, and the following guidelines assume that air bending is to be used. Air bending uses the minimum amount of force, which maximises the capabilities of the pressbrake and minimises wear on the tooling.
With air bending, the inside radius is predominantly determined by the die opening or V-width. It is preferable for any given material to use the largest practical die opening to minimise the force required, which results in a larger radius. Often a smaller radius is desirable and a good rule-of-thumb is to use a minimum inside radius equal to the material thickness. Dies are manufactured in particular sizes and this limits the choice of radii for a particular material. For this reason generous tolerances on the inside bend radii should be allowed for in the design (typically +/- 30% of the required dimension).
Folding aluminium can be difficult as it has a tendency to crack, particularly when bending parallel to the material grain. Softer alloys such as 1050, 3103, 5083 and 5251 are less problematic and can be folded in a similar manner to mild steel. Harder alloys, such as those in the 2XXX series, may require minimum bend radii between four to eight times material thickness to avoid cracking.
The recommended minimum flange length would be at least four times the material thickness. The limit on small flanges obtainable on the pressbrake is determined by the die opening or V-width. Small flanges approach the edge of the die opening and can slip under the top tool as it penetrates. This makes it physically impossible to produce the bend in one operation. A smaller flange is only possible with additional work, such as forming a larger flange and then machining to size, which makes it a costly feature.
If a bend is too close to material on an adjacent edge the material is likely to tear. Part A illustrates the problem. To prevent tearing, either the bend to edge distance should be increased, as in Part B, or bend relief should be cut into the part, as in Part C. The relief length should be greater than the radius of the bend and the width of the relief should be at least the material thickness. Bend relief has a number of benefits. The bigger the relief, the easier it is to align the component over the tooling reducing both setup and running costs.
Relief also prevents crack propagation which is particularly important if the component is subject to vibration as existing cracks can grow rapidly. In these situations it is best to avoid creating relief with sharp corners so that that finished component will be more durable.
It is recommended that holes are positioned away from bends to avoid distortion. If a bend is too close to a hole, the hole would become deformed during the bending operation. A hole required so close to the bend would therefore need to be created after bending with a secondary drilling operation. To avoid this additional expense, any holes or slot edges can be positioned so that they are clear of the die opening when the bend is formed. As a rule-of-thumb this equates to a distance three to four times material thickness from the bend line.
The opposite picture illustrates the distortion created at the edge of a bend as material thickness increases and bend radius decreases. If this distortion is unacceptable then the component can be relieved as shown in the picture.
When designing sheet metal components with folds or bends it is necessary to create a flat pattern or blank development of the part. This blank is then laser cut or CNC punched before arriving at the pressbrake for folding. In creating the blank, it is important that the design takes into account the bend radius formed by the pressbrake tooling. The bend radius has the effect of decreasing the developed blank size. The larger the radius, the smaller the blank, as shown in the example oppsite. The design calculations required for sheet metal blank development are referred to as a “bending allowance” calculation.
The bend radius varies with the material thickness and the tooling used for bending the material, and each subcontractor will have their own tooling preference, meaning that different subcontractors may use different blank developments. It is therefore essential that the production designer or engineer is aware what tooling will be used to bend the material and have a good appreciation what affect this has on the bend radius, and the resulting blank development size. Likewise, to ensure accuracy of the bent component, the pressbrake operator needs to know what radius the part has been designed with so that the correct tooling choice is made.
Dimension the part in a single direction where possible. Due to the sequential nature of the forming process, and the fact that a dimensional variation is introduced at each bend, dimensioning in a single direction parallels the process and helps to control tolerance accumulation.
Allow a more generous tolerance on flange lengths (+/- 0.2mm) as tighter tolerances, while achievable, will make the part more expensive. Often tolerances in the drawing title block may be unnecessarily tight for certain dimensions and angles, while appropriate for others.
Avoid dimensioning bend radii where possible. Each subcontractor will have their own tooling preference, and this determines the bend radii on the part. If bend radii are important then whenever possible use the same bend radius for all of the bends on the part. This helps the subcontractor minimise set-ups and reduce costs. In any event, a generous tolerance should be allowed to allow a maximum choice of tooling (typically +/- 30% of the required dimension). Note that the resulting radius should not vary within a batch of components made with the same tooling despite the wide tolerance allowance.
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 gauges.
Outside dimensions should be used. Unless the inside dimension is critical it is preferable to use outside dimensions as these are more easy to measure. However, offsets and embosses should be dimensioned from the same side of the material unless the overall height is critical.
Only the absolutely critical dimensions should be highlighted as such. Placing excessively high tolerances and redundant critical dimensions on a drawing can dramatically increase the cost of the part.
Mark up blank developments as “For Information Only”. Developments provided by third parties are often created without consideration for the actual pressbrake tools to be used during production, which will influence the accuracy of the finished part. To maximise quality, precision subcontractors will generate their own blank development to suit their tooling, ensuring that the formed component matches the requirements.
