DANIEL FRITZINGER
Product Development Engineer
Rieke Corp.
Auburn, Ind.

 

Edited by Paul J. Dvorak

Designers who call for shaped tubing are asking for trouble when they send drawings to manufacturers with incomplete information. Designers of bent tubular components should have some background on how parts are formed, limitations of the process, and what information manufacturers need to deliver the parts designers expect. The following rules can help fill gaps in a designer’s knowledge base when it comes to designing or specifying formed metal tubing. Though the rules also partially apply to metal rods, they need a few additional guidelines not covered here.

Understanding how manufacturers bend tubes provides a first step to better parts. Tube benders are usually made of three dies — a forming die, clamping die, and pressure die.

The forming die determines the tube’s bend radius. Tool manufacturers usually stamp the die with its bending radius and tubing diameter. The radius marked on the die usually indicates a radius to the centerline of the tube. Additionally, toolmakers usually scribe the forming die with a tangency line to indicate the transition between the straight and curved portions of the die.

A clamping die holds the tube tightly against the forming die so the tube does not slip during forming. And the pressure die holds the tube in position as it feeds in and pulls around the forming die.

Designers usually know the material sizes (outer diameter and wall thickness) and bending dies available or commonly used by the metal fabricator. When unknown, the designer should find this information before going any further. Specifying a bend radius the manufacturer cannot produce can seriously delays projects committed to tight schedules.

A good guideline regarding bending die selection is to choose a radius at least three times the tube’s outer diameter. This usually avoids rupturing or tearing the material as it bends. For example, if using a 0.75-in.-OD tube, the bending radius should be at least 3 x 0.75 = 2.25 in. The three-times rule, however, is only a guideline. Several successful designs sport bending radii less than three times the material OD.

After choosing material size and bending dies, layout the overall shape of the part. Now the designer can generate the production information needed by the metal fabricator. The drawing should contain at least the following elements:

Material identifier, 1020 HR steel or T6061 for example, along with the material’s OD and wall thickness.

Radius of bend is usually governed by the space the part must fit, the dies available to the fabricator, and the 33 OD guideline.

Bend angle is the number of degrees the material bends. Although the angle sounds like a simple measurement, it is important that designers understand the concept because it greatly affects raw material calculations. More than one designer has miscalculated raw material length because the angle of bend concept was improperly understood.

Length of bend is calculated from the previous information. It is nothing more than the equation for the length of an arc. Remember that it is based on a bending radius through the centerline of the tube or rod. Mechanical theory suggests that as a material bends, material fibers outboard of the centerline stretch, while material fibers inboard of the centerline compress. Fibers at the centerline remain unchanged. To find length, use

L = 0.01745ur where L = length of bend, in., u = angle of bend, degrees, and r = radius of bend, in. The constant is a conversion from radians to degrees.

Raw material length applies to straight stock. Once the location of all bends and lengths of bends are determined, the designer can calculate the raw-material length. This is also the fabricators cut-off length. The calculation is simply the sum of the lengths of the straight and bend sections.

Assign final part dimensions with appropriate tolerances. At this time the designer can finish the part drawing by applying the dimensions used to inspect the part after it is fabricated. These dimensions are not necessarily the same used by the fabricator to make the part. Finding the bend location using the point of tangency is an essential setup dimension for the fabricator. However, it is difficult to accurately measure the point of tangency after bending the tube.

With regard to tolerances, evaluate the design for the largest tolerances that will still let the part function. Welding fabricators often bend and twist widetolerance parts into welding fixtures when the part goes into a larger frame. Fabricators can suggest tolerances their bending machine can hold. Benders can run the gamut from small bench top hand benders capable of holding a few degrees to large CNC benders capable of holding much tighter tolerances. Also ask the welding crew how much bending and twisting they are willing to impose on parts.

Lastly, it’s a good idea to cut the raw material for first-piece prototypes slightly longer than the calculated raw material length. When all goes well, the straight section of the part located beyond the final bend will be slightly longer than spec and can be trimmed to make a usable part. But should the initial bends use more material than expected, a longer-than-calculated length of raw material hopefully provides enough tubing to still make a usable part. In either case, the print can be updated after verifying the raw material length.