Designing in Plastic, Part 217 May, 2004 By: Adrian Scholes
Solid Edge helps generate parts that are manufacturable and functional
Last month, we looked at Solid Edge's flexible shape- (or form-) creation capabilities for designing plastic parts such as those common in consumer products. This month, we explore different modeling approaches and plastic-specific features you can use to add function to your plastic parts.
I can't overstate the value of open profiles for modeling plastic parts. Open profiles let you construct features that intersect and blend with desired faces, or intersect multiple faces, without protruding through the part wall. When you construct a feature that has an open profile, the profile's ends extend toward the existing model's intersections. Lines extend linearly, arcs extend radially, and material is added or removed along the extended profile's full length in the selected direction. Note that you're not adding elements to the profile to close it. This is especially useful when you change the original features or faces - because the open profile remains open, it updates correctly to maintain the feature.
DRAFT ANGLES AND CROWNING
Plastic parts almost always require draft angles to make the part easier to remove from the mold. Also, a more aesthetic form of draft - a crown, which adds curvature to the drafted face - can improve the finished part's appearance and physical properties (figure 1). You can apply draft angles or crowning to the faces of features created using the Protrusion, Cutout, and Extruded Surface commands. If you define a symmetric or nonsymmetric extent using any of these features, you can define individual draft or crown parameters for both extent directions. The Crown Parameters dialog box allows you to specify the crown type and parameters. You can either define a radius for the full extent of the crown or key in an offset dimension where you want the curvature to begin. You can also define an angled takeoff, which provides a greater degree of apparent draft angle leading up to the curvature. Finally, use the Flip Curvature option to create a concave or convex crown.
Figure 1. Drafting and crowning features help you meet aesthetic requirements while building in manufacturability.
Most plastic parts consist of an external shape that is hollow to accommodate internal components. Usually you achieve this by constructing a solid feature and then using the Thin Wall command to create a wall of the desired thickness. This approach works well until you need to add downstream features that require the same wall parameters. Reordering the feature tree doesn't always achieve the desired results and may even cause the model to fail. The Thin Region command overcomes this, allowing you to carry out a controlled thin-wall operation on a selected region of a part. The process is very similar to that of the standard Thin Wall command. Begin by selecting the faces you want to thin. These faces will form the "walls" of the new feature, using a common thickness and any unique thicknesses you define. Next, select any faces you want to leave open.
The command's real power is its ability to define capping faces. You can use any face or construction surface to define how you want to cap the thinned region. You can use a capping face with or without an offset, each producing a different effect (figure 2). When you specify a capping face with no offset, the software extends the face to cap the bottom of the thin region.
Figure 2. The middle rectangular boss used the red capping face to create the thin region with no offset. The right-hand circular boss included an offset.
RIBS AND WEB NETWORKS
Because plastic parts are often hollow and thin, designers typically strengthen them with ribs and web networks, some of which double as mounting features. Solid Edge's Web command creates a rib network complete with any desired draft angle. The command also takes advantage of open profiles. If the profile you draw doesn't connect to a part edge, you can choose to keep the rib or web element a finite length or extend it to intersect with existing part faces.
The Boss command is a Solid Edge super feature - a single command that replaces what would often require creating multiple profiles and features. Typically used for mounting bosses, this command constructs a simple cylindrical boss. You can specify Center Hole, Stiffening Rib, Draft Angle, and Rounding parameters, all of which the system adds at the time of creation and which you can easily edit later using the same dialog. One command adds multiple bosses. You don't have to manually draw a profile for a mounting boss; just specify the desired properties using the Options dialog box and position the profile. Because the mounting boss rarely sits on a planar surface, you define the profile plane above or below the surface toward which you want the boss to extend. If the boss has stiffening ribs, you can also use the dialog box to rotate a profile to a different orientation. When a mounting boss feature consists of multiple profiles, you can define a unique rotation angle for each profile in the feature.
Another super feature, the Vent command constructs a cooling vent-type characteristic using a single dialog to define the exterior boundary, ribs, and spars along with rib and spar properties such as thickness, depth, draft, and rounding (figure 3). You also can specify whether the ribs or spars extend past the opening created by the boundary element and whether the ribs or spars are offset from the entrance surface. Construct a vent feature by selecting elements from an existing sketch and projecting onto a surface. The vent maintains the surface contour. If the surface is cylindrical, a section through the vent shows that it follows that cylindrical profile.
Figure 3. A single sketch defines the many attributes of this cooling vent, which is placed using one command.
Most consumer-type plastic parts have a finished shape that consists of multiple parts. A telephone handset design, for example, typically begins as a vision of a single aesthetic shape, but engineering and manufacturing constraints necessitate multiple parts joined together. Solid Edge's Divide Part command allows you to think and work the same way. Use traditional solid and surfacing commands to create the finished form, then divide it into parts using reference planes or construction surfaces to define each split (figure 4). The Divide Part dialog box defines new names for the resulting parts. Each part remains associative to the original part document so you can continue to work with the overall shape and know that the software will update the parts accordingly.
Figure 4. You can define the overall shape of a part and then divide it into associative elements. Then you can add lip/groove, web, and other features to the divided parts.
Continuing the theme of joining, most plastic parts use a lip and groove arrangement to create a smooth joint that hides any minor design discrepancies. Traditional sweep commands can twist the profile to give inaccurate results. You can prevent this by using Solid Edge's dedicated Lip/Groove command. Simply specify an individual edge or chain of edges and type in the height and width for the feature. The system dynamically represents the feature, and you simply move your cursor to position it to add or remove material as required.
SUCCESS INSIDE AND OUT
For designing plastic parts, Solid Edge is the most efficient product on the market, providing flexibility and plastic-specific features not found elsewhere. By combining Solid Edge's Rapid Blue technology (see April's column) with the process-specific capabilities discussed here, you can explore different approaches to your plastic part modeling, so that when you change the outside shape, the internal engineering features update correctly and retain the desired technical functions.
See you On the Edge next month.
About the Author: Adrian Scholes