June 1, 2008
Columnist Gerald Davis reveals the usefulness of unfolding parts on the computer screen.
Three-dimensional CAD software provides great power to generate flat layouts of sheet metal parts with just a click of a button. But as Uncle Ben told a young Peter Parker in Stan Lee's "Spider-Man" saga, "With great power there must also come great responsibility."
So what responsibilities should CAD jockeys take on when it comes to flat layouts?
Over the past few years, I have asked dozens of sheet metal shop operators the following question: "Do you generally ask your customers to supply you with flat layouts generated by their 3-D CAD systems?" With only a few exceptions, the answer I have heard to this question is "Heck, no!"
The general reason for this dim view of computer-generated flat layouts is that the accuracy of the calculation heavily depends on the specific tooling used to form the parts. Some general formulas give a reasonably good theoretical prediction, but those formulas are based on perfect radii and ideal tooling and material condition. Each manufacturing shop has its own secret set of time-proven methods for calculating flat layouts.
The idea of training customers how to calculate the perfect flat layout just does not make sense to many job shop owners. In their opinion, as manufacturing craftsmen, they bear the responsibility to create the flat layout. It is the customers' responsibility to generate the design that is to be manufactured.
In combination as a team, design and manufacturing can produce wonderful products. There is no need for duplication of effort.
Without disputing the notion that manufactured quality and accuracy are the purview of those building the parts, the manufacturing department must understand that real benefits can be realized if the designer knows something about the shop floor. We will examine three specific examples of how a design can be improved by considering the flat layout in a moment. Before that, however, we should cover the basics of flat-layout calculation.
Suppose that every time you bend something, it stretches. In fact, every time you bend the same material in the same way, it stretches by the same amount. What impact would that have? If your goal is to make a thing that is just the right size, you'd have two options. One is to trim the part after you form it. The other option is to start with a smaller piece of material in the flat and take advantage of the stretching to achieve a part that is the right size after it is formed. That's a little bit of a simplification, but that's also the secret behind flat-layout calculations.
The simplification I just made was to gloss over the way that the formed part is measured. In general, if the part lengths are measured on the outside, then the part does indeed appear to stretch as it is bent (see Figure 1). On the other hand, if the measurements are taken on the inside lengths of the part, then a different result emerges—so different, in fact, that it appears the material actually shrank instead of stretched.
For many years professionals in the sheet metal trade have used bend deductions to compensate for stretching when using outside dimensions shown on design drawings. They use bend allowances when calculating with inside dimensions. In other words, they deduct (by subtracting) from the flat length when they expect it to stretch; conversely, they allow (by adding) for any expected compression of the metal.
The amount of the deduction or allowance depends on the bend radius, the bend angle, the material thickness, the material stiffness, the tooling used, and how much contact the tooling makes with the metal. In an extreme situation, tooling may coin the material by pressing so hard as to swage the material into the bent shape. At the opposite extreme, the forming process may leave air gaps between the tooling and the workpiece except for the necessary contact points to cause bending to occur.
Somewhere between the outside (the stretching) of the part and the inside (the compressing) of the part is an imaginary neutral line that does not change length while the part is being bent. The neutral line does move, however:
The distance from the inside of the part to the neutral line can be measured as a ratio (like a percentage) of the material thickness. If the neutral line is exactly halfway into the material, that would be 1/2 or 0.5000. If the neutral line was 3/8 of the way into the material, the ratio 3/8 would be expressed as 0.3750, and so forth.
This esoteric ratio for locating the imaginary neutral line commonly is referred to as the K factor (see Figure 2). The remarkable thing about K factors is that they work for practically any bend angle. Remember, bend deductions and bend allowances are specific to a bend angle.
If you know the material thickness, the bend radius, and the material stiffness, you can know a single K factor that will work no matter what bend angles are involved in forming the part.
Humans enjoy bend deductions and bend allowances because they work nicely with calculators; they are easy to predict and confirm. CAD systems prefer K factors because they are universal and efficient for the software programmers to code. If you asked a human to use a K factor to generate a flat layout, the person probably would fuss over the extra work required, especially when compared to just subtracting a deduction known by heart. The dumb computer program would have to look up the deduction from a table every time it encountered a bend. Table lookups are slow and complex for a computer program (as compared to just multiplying a constant).
The result for CAD jockeys is that their software systems will work great with K factors. That's the good news. The bad news is that very few press brake operators will use K factors; instead, they'll use the traditional bend deduction or bend allowance.
Fortunately, it is not that hard to convert the traditional deduction or allowance into a K factor. CAD jockeys can be happy with one arithmetic method; manufacturers can use theirs. Theoretically, both will arrive at the same final answer no matter which calculation technique is used.
What anyone must know to do a flat-layout calculation correctly are the bend radius, gauge thickness, and the material's yield strength. It is then a matter of personal choice whether to use a K factor, a bend deduction, or a bend allowance.
Numerous online sources can be consulted for detailed discussion of flat-pattern calculation. A quick Internet search will give you plenty of ammunition for defending your preference in calculating a flat pattern. The point I want to leave you with is that most CAD systems use K factors and most humans use something else.
One of the small joys in my life as a cost estimator was opening up a drawing for a product that defied the laws of physics (see Figure 3a). It was always kind of fun as a simple-minded sheet metal mechanic to humble the brilliant CAD jockey with a dose of reality.
As you study Figure 3a, you'll note the bends on all four edges of the bottom floor. The front panel has four slots for mounting. Stiffening flanges sit behind the front panel and have matching slots with the front panel. The design intent is for the clamping action of the mounting screws to stiffen the entire frame during installation.
Figure 3b reveals why I guffaw at this design. The design details two areas where the sheet metal has to be in two places at the same time, which is a physical impossibility.
This example is a good reason for CAD jockeys to know how to generate flat patterns. By unfolding the part on the computer screen, the designer can see the problem revealed and correct it before it is sent to manufacturing. A possible solution is shown in Figure 3c. By removing the wings on the front panel, the part can be unfolded. Some other component or weld might be required to achieve the target installation rigidity.
Figure 4a shows our next reason for mastering flat layouts. The chassis is made from 0.062-inch 5052-H32 aluminum. Our design calls for an interior cutout that has flanges around its perimeter. Figure 4b shows the flat pattern. I've turned off the bend lines to emphasize what the cutting requirements are. The four diagonal slots are 0.037 in. wide.
Those narrow diagonal kerfs create a couple of problems for manufacturing. First, it is less than the 0.062-in. material thickness, which is forbidden when punching a part. Second, if the part will be fabricated using a metal cutting laser, then this design might benefit from having a narrow slit on the order of 0.008 in. wide.
As background information, my manufacturing department has given me the ideal bend deduction (which I translated into the perfect K factor of 0.4844). I know that my flat layout is correct. I also know that I want this part to be fabricated using a punching process, so I'm going to adjust the design to use available 0.090-in.-wide slitting tooling. The result is shown in Figure 4c. The aesthetic impact is minimal, but the result is a part that is much easier to manufacture.
Figure 5a shows a dimensioned flat pattern for a sheet metal part. The overall width is 12.044 in. In the U.S., a common flat sheet size width is 48 in. If a 48-in.-wide sheet of raw material is used, manufacturing will be able to nest only three parts in that width.
If we asked the CNC programmer what a better size for our chassis might be, the answer would probably use the following reasoning: "We want a border region for the shaker frame—something on the order of 1 in. We could common-edge punch the parts with a 0.250-in.-wide slitting tool." The short answer is that we should try to keep our flat size somewhere around 11.312 in. if we really want to make the best use of raw material.
Figure 5b shows the result of trimming about 0.732 in. from the width of our design. Manufacturing now can nest four parts in a 48-in. width of raw material. In this example, we get five parts for free compared to what we got before. If the design can tolerate the smaller chassis, we've done an excellent job of cost reduction.
In this example, it helps if the CAD jockey is armed with the perfect K factor, but just using a default K factor of 0.5000 (instead of 0.4844 in this example) would get the job done as well. Manufacturing could adjust the 1-in. shaker frame width to suit.
Keep in mind that this article has addressed general recommendations. It is very important that design and manufacturing people communicate with each other to nail down the specifics about whether or not a flat layout is desired, what the right K factor should be, and what the recommended inside bend radius is for various alloys and gauges. They also need to discuss material grain direction, tooling marks, and available tooling.
Gerald would love to have you send him your comments and questions. You are not alone, and the problems you face often are shared by others. Share the grief, and perhaps we will all share in the joy of finding answers. Please send your questions and comments to email@example.com.
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. Print subscriptions are free to qualified persons in North America involved in metal forming and fabricating.