Working with Sheet Metal Parts in Solid Edge1 Aug, 2003 By: J. Fred White
The Sheet Metal environment in Solid Edge provides a set of commands tailored for the efficient construction of sheet metal parts. Sheet Metal is not a standalone product; it is an environment within Solid Edge, similar to Solid Edge Part, Assembly, or Draft.
You construct a sheet metal part by constructing a base feature and then adding features until the part is complete. Sheet metal properties such as material thickness, bend radius, and bend relief are easy to control and manage. Instead of defining these properties each time you add a new feature, you can use the default property values provided in the template.
The Base Feature
You can construct a base feature with the Tab, Contour Flange, or Lofted Flange commands. The Tab command allows you to construct a flat feature of any shape using a closed profile. The Contour Flange command allows you to construct a feature comprising one or more bends using an open profile. The Lofted Flange command allows you to quickly construct a flange using two open profiles on parallel reference planes. Like the Contour Flange command, the Lofted Flange command automatically adds bends using the bend radius property. You do not have to draw an arc at each bend location.
The Part Properties tab on the Options dialog box allows you to set up the sheet metal properties for the part you are constructing. These properties are copied to the Variable Table and reused each time you create a new feature. For example, when you construct a flange, the material thickness and bend radius are automatically applied.
If you edit these values later, the part will update. For example, if the material thickness for the part needs to be increased, you can edit the value for the material thickness, and the material thickness for the entire part will change.
Adding Features. After you have constructed the base feature, you can use the commands on the Sheet Metal Features toolbar to complete the part by adding features such as flanges, cutouts, holes, louvers, beads, and so forth.
Feature Properties. You can also change the properties of an individual feature. For example, you may want to use one bend radius value for the entire part, except for one flange, which needs a larger bend radius. Select the flange you wish to edit and click Flange Options on the ribbon bar to change the bend radius property.
Bend Relief and Corner Relief. When constructing and modifying flanges and contour flanges, you can use the Flange Options dialog box to control whether bend relief or corner relief is included as part of the feature. If you define a bend or corner relief, you can also control the size and shape.
The bend relief specified is applied to the source face from which the flange is constructed. For example, when constructing a partial flange centered on an edge, bend relief is added to the source face on both sides of the flange.
Figure 1. The corner relief options available are None (A), Bend Only (B), Bend and Face (C), and Bend and Face Chain (D).
You can also use the Extend Relief option to specify whether the bend relief is applied only to the area adjacent to the bend or to the entire source face. As shown in Figure 1, you can define the following options when applying corner relief:
- Bend Only(B)
- Bend and Face(C)
- Bend and Face Chain(D)
Closing Corners. The Close Corner command will modify two flanges in one operation to close the corner where the two flanges meet. Since closed corner is a treatment, you do not have to draw a profile--just select the edges you want to modify.
Mitering Contour Flanges. You can miter the ends of a contour flange by setting options on the Miter 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.
Adding Features across Bends. On many sheet metal parts, cutouts or holes lie across a bend. You can use the Unbend command to flatten a flange so you can add a feature, such as a cutout or a simple hole, across the bend. After you add the feature, you can use the Rebend command to deform the flange again.
Sheet Metal Cutouts. When constructing Sheet Metal parts, you can construct cutouts using the Cutout command or a specialized Normal Cutout command, as shown in Figure 2. If the cutout you are constructing will result in thickness faces not perpendicular to the sheet faces (as in area A), you should consider using the Cutout command.
Figure 2. There is a difference between the Cutout command and the Normal Cutout command. For a cutout that will result in thickness faces not perpendicular to the sheet faces (A), use the Cutout command. Normal Cutout creates thickness faces that are perpendicular to the sheet faces (B).
When you use the Normal Cutout command to construct the cutout, the software creates thickness faces that are perpendicular to the sheet faces (as in area B). Although the Cutout command would successfully construct the cutout, you might not be able to flatten the part later or add features to the non-perpendicular faces. With a normal cutout, the feature would likely be manufactured while flat.
Adding Features in the Part environment
You can access a Sheet Metal document (PSM) in the Part environment, in order to add non-sheet metal features, using Switch to Part Environment. After you have finished, you can return to the Sheet Metal environment using the Switch to Sheet Metal Environment option.
You can add any type of Part feature to a sheet metal part, but some features can prevent the part from being flattened with the Part Copy command. If you intend to flatten a Sheet Metal part later, you should create a test part and see if the part features you want to add can be flattened.
Flattening Sheet Metal Parts
After constructing a sheet metal part, you may need to create a flat pattern of the part for manufacturing. You can use the Part Copy, Flatten, and Save As Flat commands to create a flat pattern of a sheet metal part.
The Part Copy command allows you to create a flat pattern of a sheet metal part in a new part or sheet metal document. The Save As Flat command allows you to flatten a sheet metal part and save the part as one of the following document types: Part document (PAR), Sheet Metal document (PSM), AutoCAD document (DXF). The Flatten command on the Simplify/Flat toolbar allows you to create a flat pattern in the same file as the formed sheet metal part.
Solid Edge supports the entire sheet metal product development process, from design of sheet metal components to flat pattern development and the creation of engineering drawings. In addition to the features outlined in this article, Solid Edge also offer integrated Voyager applications for analysis, nesting, NC programming, and related tasks.