Pro/E Versus SolidWorks
Mark Biasotti, IDEO’s top mechanical CAD expert, is one of the rare individuals who works extensively with both Pro/Engineer and SolidWorks. IDEO, a subsidiary of Steelcase Inc., is one of the top U.S. industrial design firms. So when Biasotti talks about differences between CAD systems, we listen. He provided much of the observations and analysis for this article.
Stylish consumer products are characterized by smoothly flowing lines accented by distinctive features. Such shapes typically are not created solely from analytical surfaces, such as planes and cylinders, which characterize machine elements. Instead they are crafted using b-spline curves and surfaces that give designers the freedom to create virtually any form. The free-form surfaces are combined to make a closed body, which is then converted to a solid model.
Most products are cast via injection molding (or in the case of large parts, rotational molding). To produce these parts, solid models are hollowed to make a thin shell. Then they’re split into two halves so that internal components can be installed.
At this point, internal details such as mounting lands or bosses are usually added to the inside surfaces of the shell, along with ribs that provide stiffness and allow thermoplastic to flow evenly into the mold.
Of course not all consumer products conform to this model. Major appliances and many computers are still made from flat sheets of metal, and internal components, such as pumps, valves, and switches are designed to accomplish a function at low cost rather than for appearance. Yet, increasingly, consumers are demanding products that look cool, so even large appliances may have free-form handles and interior moldings. A CAD tool for consumer products needs to meet the demanding requirements of industrial designers.
To appreciate what enables CAD software to produce graceful flowing curves, it’s important to understand some concepts of continuous curvature. The curvature of a curve or surface is the inverse of the radius of the curve at each point along its length. An arc, circle, or cylinder has a constant curvature as does a straight line or plane whose curvature is zero. When a circular fillet is tangent to a straight-line segment, the curvature falls abruptly from a constant value to zero.
The human eye can perceive abrupt changes in the curvature of surfaces. A round fillet meeting a plane surface appears to have a ridge at its edge, even though none physically exists. Artfully designed products thus avoid discontinuities in the derivative (rate of change) of the curvature of curves and surfaces except where ridges and sharp edges are used for accent. Entities whose curvature derivative is continuous are said to be C2 (or sometimes G2) continuous. Curves and surfaces that are tangent are said to be C1 (or G1) continuous, while continuous curves or surfaces with sharp edges are said to be C0 (or G0) continuous.
Most CAD systems can produce curves and surfaces that are continuous (C0) or tangent (C1). However, only the best systems can produce surfaces that can be joined with C2 continuity under a wide range of conditions. Pro/Engineer Wildfire maintains C2 continuity between adjacent surfaces under more conditions than SolidWorks 2004.
Curves are the basis of all free-form surfaces. A CAD system with inferior tools for creating curves will invariably produce poor-looking surfaces. So before comparing the surface-building capabilities of Pro/Engineer and SolidWorks, it’s worth looking at their ability to generate curves in three-D space.
Both Pro/E and SolidWorks can construct 2D sketch profiles using splines and analytic geometry such as lines, arcs, and conic sections. Both also can construct curves through three-dimensional reference points that are either fixed in space or attached to existing part edges or vertices. Where the two programs differ is that Pro/E Wildfire has the ability to adjust curves with sliders and then assign tangency and C2 matching to existing model surfaces, solid faces, and edges. SolidWorks can’t assign tangency or C2 matching at curve endpoints.
SolidWorks can build 3D curves using what it calls a 3dsketch. This type of sketch is in some ways more versatile than Pro/E’s ability to draw curves thru points because users can combine both analytical entities and splines into a single feature. SolidWorks users also can dimension and constrain three-D sketches in ways that Wildfire users can’t. Unfortunately SolidWorks can’t connect 3dsketch splines end-to-end with continuous curvature.
Both Pro/E and SolidWorks can convert sketch entities to a single composite curve. This feature is important for advanced surfaces because the edges that define them must be smooth and free of multiple sketch segments.
SolidWorks does this better than Wildfire because it can convert a two-D or three-D sketch composed of multiple entities using its Fit Spline function. Unlike Wildfire, SolidWorks lets users control the deviation tolerance between the fitted curve and the original entities. This capacity gives SolidWorks the ability to skip over small gaps in the underlying geometry.
Boundary surfaces are the surface features most commonly used for creating complex shapes, according to Biasotti. As their name implies, these surfaces are constructed between three or four bounding curves in space. Competent systems enable designers to add interim curves between the bounding curves to influence the surface shape.
Pro/Engineer Wildfire’s boundary surface is called a Boundary Blend. One of its unique features is that users can dynamically adjust the boundaries — foreshortening, extending, or snapping them to references on an existing model – by dragging on the end points of the bounding or intermediate curves that define the surface.
SolidWorks does not have true boundary surfaces. Instead it approximates them with its Loft-with-Guide-Curve feature. A SolidWorks lofted surface is defined by two profiles, which may be planar or three-D curves. To control the shape of all four boundaries, guide curves may be added on the two edges not defined by the profiles.
SolidWorks’ Lofted Surface with guide curves is not the equal of Pro/E’s Boundary Blends. Profiles and guide curves don’t have equal influence over the shape of the surface. This asymmetry can cause undesirable undulations in the surface, Biasotti has found.
SolidWorks also offers designers less control over matching conditions between adjacent surfaces than Pro/E does. Although SolidWorks enables adjacent lofted surfaces to be tangent, it can’t assure continuous curvature (C2) between two surfaces, as Pro/E Wildfire can.
Swept surfaces are another commonly used feature in industrial design. Sweeps resemble lofted surfaces with guide curves, except only one profile is swept along a trajectory.
To create complex shapes, additional features have been added to the basic swept surface to give designers more control. Pro/E Wildfire has what is called a Variable Section Sweep. This most powerful feature sweeps a profile along a path and allows the designer to define multiple paths (often called guides or rails) that constrain the profile to follow them. The guides alter the length and shape of the swept section as it follows the path.
Additionally, designers can assign a pivot direction to variable section sweeps to ensure that the initial profile does not twist or contort as it moves along a three-dimensional trajectory. Biasotti says this pivot direction is invaluable for building surfaces that need to be drafted by a certain degree at all points along the path so the part can be molded.
Another feature that makes Pro/E’s Variable Section Sweep exceptionally powerful is the ability to assign either tangency or C2 continuity to guide curves on the edge of an existing surface or solid face. This control enables designers to blend a swept surface with another shape while assuring a flawless transition between them.
SolidWorks also has the ability to control swept surfaces and solids with guide curves, giving it a capability similar to Pro/E’s Variable Section Sweep. An unlimited number of guides can be used with the path and profile. SolidWorks has diagnostics for determining where the sweep fails along the path, a valuable tool for anyone using this feature.
Unfortunately, SolidWorks can’t make guide curves tangent or C2 continuous with adjacent surfaces, as Pro/E can. SolidWorks basic sweeps have a Path Alignment option that works similarly to Pro/E’s Pivot Direction. Unfortunately Path Alignment only can be used with unguided sweeps. As soon as the designer selects a guide curve, the path-alignment option disappears from the menu. In summary, SolidWorks’ swept surfaces and solids are more limited in their capabilities than Pro/Engineer’s.