Design tips for sheet metal: Bend relief, small holes, hole distortion near bends, and minimum flange widths
The article discusses making small holes and when to use a punch or laser cutter, inside radius measurements and how they differ depending on whether you are coining or air bending on a press brake, and adding bend relief to prevent tearing material.
My experience, and therefore this article, is limited to sheet metal for applications such as power supplies, dispensing mechanisms, and electronic enclosures.
I run a job shop. We need maximum tooling and machining versatility, so tooling dedicated to a specific product is used only when absolutely necessary.
The punching equipment that we use generally limits the smallest hole size to be equal to the material thickness. This constraint is a result of punch tip strength. If the diameter becomes too small, the punch bends or breaks before it can be pushed through the material. If smaller holes are required, we can cut them with a laser.
Determining the smallest inside bend radius is harder than determining the smallest hole size because it depends on both the workpiece material and the process used to produce the bend.
The more ductile the material is, the smaller the bend radius can be. In general, the inside radius should be at least equal to the material thickness. We are talking about mild steel sheet metal between 0.02 and 0.13 inch.
When setting up our press brakes, we have a choice of coining, bottom bending, or air bending. Coining uses enough tooling pressure to cause the workpiece material to flow into the final configuration. Bottom bending causes the tooling to contact the workpiece fully but uses slightly less pressure. Air bending uses the minimum amount of tooling contact and pressure.
When coining mild steel, the inside radius can be nearly zero. With air bending, the inside radius is controlled largely by the V-die opening; the "normal" range for the radius is one to two times the material thickness. Many job shops have an inventory of press brakes featuring several bend radii. The common increment between these radii is 1/32 inch. Keep in mind that the radius won't vary from part to part but may change from batch to batch.
We are pleased when drafters specify bends in a manner that allows easy tooling selection. We suggest that when the design calls for it, drafters specify the bend radius with a tight tolerance. Otherwise, we advise drafters not to dimension the bend radius at all.Aluminum tends to crack, particularly when bending parallel to the natural material grain. Softer alloys, such as 3003 or 5052, can be bent about the same as mild steel. Stiffer materials, like 6061 or 2024, may require four to eight times the material thickness for the minimum inside radius.
When sheet metal makes a transition from a bend to a flat surface, or to another bend, it tends to rip and tear. To eliminate this, a bend relief is added so the edge of the sheet metal is perpendicular to the bend. In general, a minimum bend relief is equal to the material thickness plus the inside bend radius. If it is OK for the metal to rip, the minimum bend relief is zero.
One benefit of a bend relief is that it makes the part easier to produce. The bigger the bend relief, the easier it is to align over the end of the tooling. The bend relief eliminates some burrs and sharp points. Without a bend relief, the part may slip unpredictably in the tooling as the bend is made.
Another benefit of a bend relief is fracture propagation reduction. If the part is subject to vibration or flexure, existing cracks may grow rapidly. By eliminating the cracks before cutting, and by cutting the bend relief with curves instead of sharp inside corners, the finished part will be stronger and more stable. I think a bend relief makes the part more attractive.
A feature that is punched near the bend line may turn into an unintended bend relief. To minimize hole distortion near bends, keep the edges of holes at least two times the material thickness away from the start of the bend radius.
A final bit of general advice: Keep the flange width at least equal to four times the material thickness. When it gets smaller than this, the tooling tends to emboss mars into the surface of the workpiece. Even worse, the operator may have to use a disposable backup strip to force the bend, or the flange may have to be milled to size after forming.
The FABRICATOR is North America's leading magazine for the metal forming and fabricating industry. The magazine delivers the news, technical articles, and case histories that enable fabricators to do their jobs more efficiently. The FABRICATOR has served the industry since 1971.