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Solid Edge

On the Edge: Using Solid Edge to Speed Up Sheet Metal Design, Part 2

14 Mar, 2005 By: Russell Brook Cadalyst

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Sheet metal treatment features give you a range of options to improve your designs.

In last month's article (click here for archives), I covered efficient use of Solid Edge's process-specific sheet metal methods and the theory behind sheet metal design. This month I want to keep the theme on sheet metal and look at treatment features, their wide range of options and the impact they have on the design. Solid Edge helps engineers speed up their design process by offering tools designed to complete a specific task, rather than a few tools, that when combined end up with the desired geometry.

The Solid Edge approach to development is to work with engineers and to find out how they work and what the end result is that they are trying to achieve. Solid Edge sheet metal is a prime example of this, meaning that engineers can focus on their design intent, leaving Solid Edge to deal with details such as bend radius, bend relief and corner conditions.

As we discussed last month the sheet metal design parameters are set in the File Properties, under the Tools / Options / Part Properties dialog box (figure 1). These settings control the material density, thickness and bend radius. The default values for bend relief, depth and width can also be set here. These are the global settings that will be applied to the model.

Additional settings can be applied to flanges on an individual basis or they can be saved as the default (figures 2 and 3). These settings can also override the default values set earlier for bend radius and relief values. Depending on how the parts will be manufactured, a round or square end condition can be chosen for the bend relief. Other options outlined in more detail to follow are settings for extending the bend and corner relief.

Corner and Bend Relief
When constructing and modifying flanges and contour flanges, it is possible to use the Flange Options dialog box to control whether bend relief (figure 4a) or corner relief (figure 4b) is included as part of the feature. If you define bend or corner relief, you can also control its size and shape.

When specifying bend relief, it is applied to the source face from which the flange is constructed. For example, when constructing a partial flange that is centered on the selected edge (figure 5a), bend relief is added to the source face (figure 5b) on both sides of the flange.

Use the Extend Relief option to specify whether the bend relief is applied only to the area adjacent to the bend (figure 6a), or to the entire source face (figure 6b).

When specifying corner relief, it is applied to the flanges adjacent to the flange that is being modeled (figure 7).

It is possible to define the following options when applying corner relief (figure 8). Further treatments can be applied using the Close Corner command, discussed later.

The various flange options provide designers with many different ways to automatically describe how both corner and bend relief should be designed to provide the best conditions for manufacture.

Profile options
By default the standard flange options yields a rectangular profile (figure 9). As we know, additional features can be added to provide cut-outs, holes, chamfers and so forth. It is also possible to change the default profile in order to add more detail, as I discuss below. This is an ideal approach for details such as slots and profile adjustments, saving both time and the need to add features.

To edit the profile simply choose the Flange feature from the pathfinder or right-click the feature and choose edit profile (figure 10). The profile can now be edited just like any other profile. Additional 2D elements, such as lines, arcs and curves, can be added, as I'll illustrate below. The only caveat is that the profile element that connects to the sheet metal body must be connected to the Connect line (figure 11).

Tip: sheet metal profiles explained. As shown here (figure 11), in order to make it simpler to construct the new profile properly, two additional dashed lines are displayed along with the default flange profile: a connect line (figure 11a) and a construction line (figure 11b).

The connect line is used to connect the ends of the flange profile to the part edge from which the flange originates. The connect line and the construction line define an area that must not be intersected by arcs that are part of the new profile. If you use an arc as part of the new profile, it can touch the construction line, but it cannot fall inside the area between the construction line and the connect line. The end segments of the new profile must be lines and they must touch or extend past the construction line.

Sometimes it is desirable to disconnect the end profiles (figure 11) to either move its position or alter its profile shape. If this is done, the end of the profile must be connected to the connect line. This can be done manually, be sure to choose the connect line and not the construction line. The easiest way is to just drag the line up past the connect line, as shown (figure 12), then finish the profile. Solid Edge will automatically trim the line and connect it. Dimensions can be added for additional control.

Sheet Metal Cutouts
When constructing sheet metal parts, you can construct cutouts using the Cutout command or the specialized Normal Cutout command. If the cutout you are constructing would result in thickness faces that are not perpendicular (figure 13a) to the sheet faces, you should consider using the Normal Cutout command.

When the Normal Cutout command is used to construct the cutout, Solid Edge creates thickness faces that are perpendicular to the sheet faces. (figure 14a).

Although the Cutout command will successfully construct the cutout, it might not be possible to flatten the part later or add features to the nonperpendicular faces. A Normal Cutout feature also better reflects that the feature would likely be manufactured while flat, when it is folded.

Adding Jogs and Bends
Using the Jog command, it is quick and easy to offset a face to any given depth. All that is required is to draw a line onto the face that is going to be jogged. Then show Solid Edge which side of the line will be offset, and finally, set a depth. When a jog is performed, material is added between the two offset faces (figure 15) and therefore material will be added to the flat pattern.

The Add Bend command (figure 16) works in a very similar fashion to the Jog command, and similar forms to the component can be achieved; however, there is one subtle difference. The Add Bend command adds a bend to the material as it is, and does not add any additional material. In this manner the flat pattern development will not change from before the bends were added. With this tool it is possible to take an existing flat pattern development or profile from another system and use reverse engineering to create a finished component.

Unbend and Rebend
The Un-bend command is intended to be used to add a cutout feature across a bend. This both eases manufacture and the design process. To unbend a flange, choose the command, then pick one or multiple bends to unbend. Create a cutout across the bend (figure 17). The cutout can partially or fully consume the bend zone.

Once the cutout has been applied, the design can be bent back to its original form. When this is done, the new cutout is considered during the rebend process (figure 18). The cutout will deform across the bend zone just as it would with the real component. During the rebending of a component (if multiple bends were unbent), they can be rebent individually or in a different order. This gives the engineers an opportunity to see if the component can be manufactured or to choose the best bend sequence.

Close Corner
As I have discussed, Solid Edge will automatically apply corner conditions. There are some circumstances where additional treatment provides more control to design engineers: There may be an awkward corner condition with a complex intersection or imported data where the design has not been very thorough. This is where the Close Corner command can be useful. It allows designs to be produced with the optimal corner and edge treatment for manufacture. Corners can be closed with either an overlapping joint or corner-to-corner condition (preferred by welders). Also, the point at which all the corners meet can have a specified treatment: They can be closed, notched or have a circular cutout (figure 19). The third option can be useful to reduce stress at the corner, which will make the component more resilient to fatigue and can make the part easier to manufacture. To close a corner, select the Close Corner command, select the converging bends to close, chose the corner treatment and finish.

Deformation Features
Last but not least are the Deformation features, which are common in many sheet metal designs. These features add a lot to the finished design, yet they are a deformation to existing faces, which means that they have little if no impact on the flat pattern. They do affect the function of the component and in some cases provide far more rigidity -- for example, using a bead to form a cross swage across a large surface. Examples of these are the process-specific features such as the Louver, Drawn Cutout, Dimple and Bead commands (figure 20).

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 allows the engineer to think about the design and leave the laborious but nevertheless important details to Solid Edge.

Solid Edge is designed by engineers for engineers, and Solid Edge sheet metal is a fine example of this. The sheet metal environment is included with every copy of Solid Edge Classic. I hope you found the sheet metal articles useful. Good luck with your sheet metal designs.

See you On the Edge next month.