Manufacturing

On the Edge: Using Solid Edge to Speed Up Sheet Metal Design, Part 1

15 Feb, 2005 By: Russell Brook Cadalyst

Understanding the available tools and the best strategy to use for the different types of design


The Solid Edge 3D design system has been developed specifically to speed up engineering design tasks. Solid Edge uses a unique situational interface, along with applied ergonomics and process-driven design tools to achieve this. One good example of this is the Solid Edge sheet-metal environment. Sheet metal is a process of designing parts of uniform thickness that usually have some kind of bend, cut-outs and deformation features. The importance of this has been recognized to the point that Solid Edge has dedicated a whole environment and suite of tools to speed up sheet metal design through to manufacture.

Solid Edge's sheet=metal environment is recognized as the most productive in its class. Many companies have chosen Solid Edge purely for its capability to design in sheet metal efficiently. Solid Edge allows them to design their components and assemblies very quickly and, once the components have been designed, easily generate an associative blank, or flat pattern.

Designing parts can be done in many ways. This article is intended to help you understand the technology behind Solid Edge's sheet-metal environment, the tools that are available and the best strategy to use for the different types of sheet metal design, whether you design simple brackets, cases for electronic equipment or guarding for machinery with compound angles.

Since Solid Edge V16 sheet-metal components can be tackled in a couple of fundamentally differing ways. The first is to start with a flat piece if material with a shaped profile or a contour flange. From this point on, other sheet metal features are added, additional flanges, holes or deformation-type features. The other is to model the component as though it is a solid component using additional part modeling features, then rip the corners to turn it into a sheet metal component. Both are very powerful ways to model sheet metal, designed to offer the best of both worlds when you need to get the job done fast.

Why is Solid Edge So Good at Sheet-Metal Design?
Solid Edge's sheet metal environment speeds up component design because it has tools that have been specifically designed for sheet metal work (figure 1). For example, the user does not have to worry about modeling bend radii, or bend relief during the modeling phase when they are generating sheet metal features. One other problem that often occurs as a design takes shape, is where the design actually gets stronger because of the inherent strength that bends and creases introduce. The design can usually be made out of a thinner-gauge material as a result; however, the internal or external dimensions will need to be altered. Solid Edge solves this problem by allowing the design to be created with critical internal and/or external dimensions in mind. If the material thickness is changed then the critical dimensions are maintained, all corresponding drawing views will also be accurately updated.

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Figure 1. Solid Edge's Smart Step' ribbon bar offers various options for sheet metal design.

Sheet Metal Options
The standard options (figure 2) are very similar to the normal part options except for two additional tabs. On the first tab, the material name can be set, material density, material thickness and bend radius (a good rule of thumb is to keep these the same; internal radius is assumed), bend relief depth and width as well as the bend equation. The second additional tab is used to set flat pattern options to aid manufacturing.

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Figure 2. Standard Sheet Metal options for designing with sheet metal in Solid Edge.

Sheet Metal Bend Characteristics
When sheet metal is formed into a bend, the metal on the inside of the bend is compressed and the material on the outside of the bend is stretched around an imaginary line along the thickness of the material sometimes call the nutral line or as Solid Edge refers to it as the PZL= Plastic Zone Length. This is important in the calculation to get an accurate flat pattern. Depending on the material, this may not be straight down the center. Aluminum is about a third of the distance from the inside of the bend because it is more malleable and stretches more than it compresses. Mild steel is usually 0.5, with harder metals, such as stainless steel, being about 0.6. This information can be gained from your material supplier. There are no hard and fast rules, and that is the beauty of the options Solid Edge provides. The neutral factor is the setting that influences the calculation to unfold the design.

Bend equation. Defines the bend equation formula you want to use. The bend equation formula is used to calculate the flat pattern of a sheet metal part. You can use the standard formula delivered with Solid Edge, one of the example formulas in the Solid Edge / Custom / Sheet Metal folder or a custom formula you develop if you need a specific override.

Neutral factor. Specifies the default neutral factor for the bends when using the Standard Formula option. This option is not available when you are using the Custom Formula option. The neutral factor value is used when calculating flat pattern size.

Standard formula. The formula used in Solid Edge is standard throughout the sheet metal industry; it uses the neutral factor, bend radius and bend angle to calculate the PZL (Plastic Zone Length, figure 3).

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Figure 3. The standard Sheet Metal bend formula in Solid Edge.

Custom formula. Folding sheet metal can be as much of an art as it is a science. In theory all the above is true and will produce excellent results in 99 out of 100 cases. However, other factors outside the design software can influence the bend characteristics during manufacture. On single bends this is not as apparent; however, a part with many bends can show incremental errors, where at least one of the dimensions can be way out of tolerance. Many sheet metal engineers who bend the components can sometimes have bend tables they have developed over time using trial and error.

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Figure 4. A custom directory in Solid Edge includes four examples of bend data tables you can use to override the standard formula.
Solid Edge can use these tables so the standard formula is overridden with sample test data from manufacturing. There are four examples delivered under the custom directory in Solid Edge (figure 4). A Read Me file explains how to use them.

If the standard automatic formula does not yield the results you require, it may be time to set up a manual override by specifying a custom formula you define to calculate the flat pattern size. "ProgramID.ClassName:" defines the custom bend formula you want to use. Type the program ID and class name using the following syntax: ProgramID.ClassName. This is explained in the Read Me file with each example.

Sheet Metal Modeling Strategy
Now that you understand how to set up sheet metal design and how the bend calculations work, and their importance, it's time to look at the two main methods of modeling sheet metal components. Both are just as productive; there is no right or wrong approach. It is not the intention of this article to cover both in detail, but rather to look at the two differing approaches so you are aware of how each works in order to choose the best method.

Convert to Sheet Metal
New to v16 is the ability to model a component, thin-wall it, then rip the corners to turn it into a sheet metal part. Engineers working on a project may also just want to reserve the space envelope on a design, before committing to the sheet metal final design at a later date. This method also works with geometry imported form other 3D design systems and is good when compound angles are required, such as in machine guarding.

Start by modeling a part using a Solid Edge sheet metal template, normal.psm (PSM stands for 'part sheet metal' it is the file format extension used by Solid Edge. This is important so we get access to the sheet metal tools. Under the File menu, choose Switch to Part. A warning will advise that features may not be properly depicted in the flat pattern (figure 5). (You wouldn't model anything that couldn't be made would you?) Model the shape that is required. You can also import a solid from another source. Don't worry about rounding the corners and so forth. Solid Edge's sheet metal tools will take care of that. Thin-wall the part and switch back to sheet metal. If you want to control where the mitred corners appear, it is possible to draw a sketch onto the model and use it to control the joint. Switch back to sheet metal.

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Figure 5. A warning will advise that features may not be properly depicted in the flat pattern.

Once back in the sheet metal environment, choose the 'Convert to Sheet Metal' command. There are two options on the tool bar (figure 6). The first converts to sheet metal and gives the option to choose which corners to rip. The second lets you rip the corners individually should you wish. A dialog box is shown with advice on how to convert the part (figure 7).

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Figure 6. The toolbar holds two options for converting to sheet metal.

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Figure 7. A dialog box offers advice on how to convert the part.

These images (figure 8) depict how a solid part is modeled as a part and then converted to sheet metal. All corners have been rounded and mitres applied.

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Figure 8. These images depict how a solid part is modeled as a part and then converted to sheet metal. All corners have been rounded and mitres applied.

It is now possible to continue to finish the model using standard treatment features in the Solid Edge sheet metal environment; we will take a look at those in a later article.

Tabs, Flanges and Lofted Parts
The second method to design sheet metal components is to use a more traditional approach. With this method the part is started using a flat sheet or a contour flange to create a base feature. To finish the design is very easy in Solid Edge -- additional flanges can be added, which automatically have the bend radius and any corner treatment already applied (figure 9). I will be discussing all the flange options in more detail next month.

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Figure 9. When you add a flange to a sheet metal design, it will automatically have the bend radius and any corner treatment already applied.

The bend radius and relief type (square or round) options are set in the Flange Options dialog box (figure 10). Here you have the choice to set the values that will be used or choose to override the default values on an individual basis to those that have been set up for the file. If no bend relief is desired it can be switched off all together, depending on design requirements and manufacturing techniques.

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Figure 10. Use the Flange Options dialog box to set the bend radius and relief type.

Contour flange. This can be used for the base feature as mentioned; it can also be used as a treatment feature -- for example, it can be used to create a metered flange around a box or electrical cabinet (figure 11). The contour flange is a very versatile tool that can be used for a host of applications.

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Figure 11. The contour flange, showing the profile and automatic mitred corners.

Mitering contour flanges. You can miter the ends of a contour flange by setting options on the Miters and Corners tab of the Contour Flange Options dialog box. For example, when constructing two contour flanges that will overlap, you can miter the ends where the flanges meet.

Chaining contour flanges. You can construct contour flanges that wrap around corners or bends. This is especially useful when constructing parts where you need to miter the internal faces of the flange, but calculating the miter angle is difficult. When you use the chain option, the miter angle is calculated automatically, and will update if the part changes. The flange profile can be straight or have curves (figure 12); bend radius are formed automatically.

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Figure 12. A contour flange with a curved profile.

Constructing hems. You can use the Contour Flange command to construct a hem, where the material folds back and touches another face (figure 13). This is sometimes known as a safe edge -- it is used to stiffen up a component, make it look nice and forms a nice clean edge. To create a hem, draw a single straight line for the profile along the face of the component -- don't leave a gap! Solid Edge will automatically create one. Choose which edges the hem will be applied to, preview the result and if you like it, accept it. Easy when you know how! Tip: Make sure you draw the profile collinear with the face on which the reference plane is based.

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Figure 13. The Contour Flange command constructs a hem, or safe edge.

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Figure 14. You can use the Contour Flange command to construct wrapped features such as this.
Constructing wrapped features. You can also use the Contour Flange command to construct features that are wrapped around a cylinder, such as in parts made by rolling perforated material (figure 14). To construct a wrapped feature, use a profile arc that has an included angle of slightly less than 360 degrees. There must be a slight gap where the ends of the rolled material meet; otherwise, the part will not unbend. Keep this in mind when defining the material side for the contour flange. Make sure the material thickness does not cause the gap to close. The easiest way to add the perforations is to unbend the part and the holes in the flattened state, and then rebend the part.

Lofted flange. Square-to-round (figure 15) and cones (figure 16) are achieved using the powerful Lofted Flange tool. It constructs a flange by fitting a feature through two open profiles. All that is needed are two adjacent profiles that are open. The best tip I can give you is that the start and end points for each profiles either line up or are the same distance away at each end, and with cones the two arcs must have the same sweep angle and at least one end must line up. This will ensure that the parts do not twist and will then flatten. The other tip I can pass on is during the side step stage, always place the material to the outside, so the profiles describe the inside sizes.

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Figure 15 Square to round design with the associative 'half' flatpattern.

The easiest way is to start by creating two sketches, rather than drawing them during the construction of the lofted feature. With the sketches in place, choose the Loft Flange icon and choose the first of the profiles, being selective of which end is the start vector. Next choose the second profile and be sure to select the adjacent start point. On the side step stage, choose to place the material outside and preview the results. A neat square to round or cone will have been constructed.

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Figure 16. A simple cone showing sweep angle of the profiles and the finished cone.

In next month's article I will be discussing in more detail some of the additional options and treatment features within Solid Edge that are specific to sheet metal design: advanced flange and flange profile options; jogs; sheet metal deformation features such as dimples, drawn cut-outs, louvers and beads; sensors, to keep a watch on critical dimensions and cost; sheet metal flat patterns both 3D and flat; and save as flat DXF for use in manufacture of parts.

Summary
Solid Edge is a powerful modeling system with process-driven tools that are specifically designed to get the job done faster. Solid Edge uses this philosophy to generate sheet metal components, which leaves the engineer to think about the design and leave the laborious but nevertheless important detail to Solid Edge.

See you On the Edge next month.


About the Author: Russell Brook

Russell Brook

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