The Best of Both Worlds
Siemens’ synchronous technology bridges the gap between 3D modeling techniques
By Ralph Grabowski | August 10, 2008
Last June, Siemens PLM Software announced the Canadian launch of its latest Velocity Series at the CN Tower complex in Toronto. While the event featured updates to all of the lineup’s packages, including CAM Express 6, Femap 10 and Teamcenter Express 4, the focus was squarely on the new history-free and feature-based version of Solid Edge.
The buzz centered on what the company calls synchronous technology (ST), a much-heralded feature Solid Edge 2008 and NX 6. A proprietary application layer built on Siemens’ D-Cubed components and Parasolid kernel, ST allows users to model parametrically, explicitly or with a combination of the two within the same environment.
To accompany the announcement, the Siemens PLM Software’s marketing department made lofty claims that had the immediate effect making some doubt their veracity. Doubt is good, and it will take months of real-life use for users to determine whether this “third way of 3D modeling” works for them.
In the meantime, mechanical CAD users are wondering: Is ST just a marketing blip or the Next Big Thing? Before exploring that question, it’s helpful to look at where mechanical CAD has come from to gain a better perspective on what synchronous technology could mean for the industry, and its users, going forward.
The History Tree of MCAD
Ever since PTC introduced Pro/ENGINEER in 1989, history-based modelers have worked in exactly the same way: they provide a rigid modeling environment in which a history tree records the details of each feature as they are created. While powerful, this strength is also its greatest weakness in that parametric packages require the designer to pre-plan a model’s construction so that parent-child relationships don’t become confused or needlessly complex. As a consequence, history-based modelers can make editing earlier in the history tree a difficult and sometimes slow process. They also have difficulty importing geometry from other CAD software.
These limitations spawned a new class of mechanical CAD programs (including IronCAD, CoCreate, Ashlar Vellum and KeyCreator, among others) that are non-history based (non-parametric). Not only are they adept at importing and editing 3D models from other CAD packages, they also allow designers to “push-pull” a model’s features without worrying whether rigid hierarchies in the history tree will break as the software recalculates dependencies.
While each technique has its upside, the difficulty has been that there wasn’t a bridge between the two camps. If you modeled explicitly, you couldn’t model implicitly within the same package. With synchronous technology, Siemens says it has spanned the gap by providing the benefits of both in the same package.
Because ST employs several interrelated concepts (including Live Rules, the Steering Wheel, 3D Driven Dimensions and Procedural Features) that differ significantly from traditional modeling techniques, it’s not easy to grasp initially. To get a better handle on how these concepts work in practice and how synchtech differs from history-based modelling techniques, I think the best way to start is with Live Rules and work through the other parts of the package to see how they interrelate.
Live Rules
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Rules currently supported by Solid Edge ST and NX 6: Concentric identifies cylindrical faces and circles with a collinear axis. Coplanar identifies faces, sketch planes, and reference planes that lie in the same plane. Tangent Edges identifies tangencies to selected elements, and then keeps them tangent through move and rotate. Tangent Touching targets tangent features, even if they don’t touch. Parallel identifies faces, sketch planes, and reference planes parallel to other selected faces, and then, and then keeps them parallel during rotate. Perpendicular locks pairs of faces at 90 degrees to each other. Symmetric About Base identifies elements symmetric about an origin; the symmetry is around the XY, YZ, and/or ZX planes. Same Radius If Possible maintains radii when models are edited. Orthogonal to Base If Possible keeps faces horizontal or vertical (not supported in NX). |
Live Rules (or Active Selection as it is known in NX 6) are used to specify relationships between features you plan to modify. As you edit the model, you click options in the Live Rules palette to tell the software which features should be affected and how.
For example, when two legs are joined by a radius, you can widen the part and the radius stays the same (the legs get wider); or you can specify that the radius increases (and the legs stay the same)— it just depends on which Live Rule you turn on.
In addition, when you select a face or feature, ST looks for all other features nearby that match those specified by Live Rules. You lock constraints to control how features change. When you modify a feature, ST alerts you to the features that will be affected. This effectively eliminates the need for traditional constraints, which I find confusing after more than a few are applied.
Naturally, you can turn off Live Rules, and you can lock down (constrain) features so that they cannot be modified.
The Live Rules palette has a second half, which kind of looks like a traditional history tree. It’s not so much “advanced” as giving you finer control over feature modification. For instance, if Live Rules picks out three planes but you want to work just with two, clicking the Advanced button allows you to deselect the unwanted plane. As you might expect, hovering the cursor over a branch highlights the features in the model to help you identify them.
Steering Wheel
While Live Rules lets you decide which faces take part in operations, the Steering Wheel (or Orient Express in NX) is a compass-like tool that lets you interface with the 3D model and control the direction in which the features move or rotate.
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The Steering WheelOrigin Knob locates the steering wheel. To relocate it, drag the steering wheel by the origin knob. Primary Knob reorients the normal; drag it to rotate features. Secondary Knob allows adjustments in 90-degree increments. Primary Axis points in the direction of the current face’s normal vector. Secondary Axis - drag to change the angle of the face or other geometry. Move Geometry - drag the blue disc to move the face and related geometry. |
The two work together like this: When a user clicks to place the Steering Wheel on a feature, the Live Rules palette appears. Check which Live Rules you wish to maintain and then drag the blue disc on the Steering Wheel to move the feature. To rotate features, drag the primary knob. Alternatively, you can also enter numeric values for distances and angles.
This kind of direct editing is possible because synchronous technology stores features in Feature Collections, where features are peers instead of having parent-child relationships, as in history-based CAD systems.
Path Finder
The closest thing in ST to a feature or history tree is the Path Finder pallet. Typically, history-based trees let you change features by editing their parameters, but you don’t do that with synchtech. Instead, to edit a feature, you work on it directly: interactively push and pull, or change the value of a dimension attached to the feature, or use the Steering Wheel. Because you can edit any part of the model at any time, synchronous technology is immensely more flexible than any history tree. While most CAD programs can directly edit models, history-based ones do this slower because the feature tree needs to be recalculated.
History-based vs. ST
Like history-based modelers, you create 2D sketches in Solid Edge 2008 and NX 6. Unlike history-based modelers, however, these ST-based CAD packages turn closed sketches into regions automatically, which you then pull and push to create extrusions—no separate Extrude command is required. The sketches disappear, presumably because Siemens thinks you no longer need them; edits are made directly with the features of the 3D model. In a similar manner, you can draw sketches on the faces of 3D models, and then push or pull them to create extrusions and cutouts. As the 3D model is built up, you edit and model with no need to worry about the order in which you create the parts.
In history-based CAD, you must always keep in the back of your mind which feature is the parent and which the child, such as holes (child) in plates (parent). Holes are created after plates, and this history governs their relationship. Consequently, these systems do not let the hole control the size of the plate; ST, however, can. You can set up dimensions that force the hole, for example, to be always centred in a plate.
“Because you can edit any part of the model at any time, modeling with synchronous technology is immensely more flexible than any history tree.”
In addition, history-based CAD requires that you apply constraints early; ST allows you to apply them earlier or later. The hole can drive the size of the plate.
History-based modelers use the history tree to record the designer’s intentions. In place of the tree, ST uses 3D driving dimensions. These dimensions can be added at any time; there is no need to place them during the 2D sketching stage.
Driving dimensions in Solid Edge 2008 and NX 6 can be dynamic or locked, or based on equations, or be linked to spreadsheets. Formulas allow you to configure parts for different size requirements. Other non-history modelers generally cannot do this.
Editing Imported Models
Non-history-based modelers are famous for their ability to import models from other CAD systems. Generally, exported models lose their intelligence, because they strip the history and parametric data, which is unique to each CAD system. Consequently, a history-based modeler has a tough time dealing with imported data; in contrast, a non-history modeler sees the unintelligent data as normal.
Synchronous technology can recapture some of the intelligence lost by collecting adjacent or related features into its Feature Collections. For example, you can import a Pro/ENGINEER model, grab a boss and add it to the Solid Edge model. From there, the boss can be interactively edited. Feature Collections understands that the boss consists of the top, sides, hole(s) and struts.
Unlike history-based modelers, you can apply constraints at any time. (History modelers usually require constraints be applied when parts—sketches, assemblies and so on—are first created.) ST allows you to add constraints later, including to imported 3D models.
History-based modeling
Although the focus in the latest versions of Solid Edge and NX has been on synchronous technology, these packages continue to be history based as well. When starting new parts, you have the option of starting with history-based modeling or starting with a ST-enabled template. While Synchronous technology also allows you to mix history and non-history parts in assemblies, you can’t use both systems in the same part. In addition, once a part or assembly enters ST “mode”, it can’t be switched back into a history-based part with its parametric intelligence in tact since synchronous technology does not maintain a history tree. Any ST part opened in parametric mode will exist purely as a “dumb” model.
At the same time, it should be noted that ST does retain the design intent of some feature types in what the software terms Procedural Features. For instance, the number of feature instances or their dimensions—such as holes, thin walls and rounds—can still be edited in the same way you would with a traditional feature tree. In addition, like history-based modelers, ST updates 2D drawings automatically as you make changes to the 3D models. Unlike history modelers, files sizes are smaller and so parts load faster.
Suggestions for Improving Synchtech
Generally, synchronous technology has met with warm reviews from the CAD blogosphere, but not without a few caveats. Deelip Menezes, for instance, suggests that Siemens add a double-click to the Steering Wheel to automatically orient it. He’d also like to see features glowing to indicate that they are affected by Live Rules as well as a preview mode that would also warns of out-of-sight features—ones that are hidden or outside the viewport.
Scott Wertel doesn’t like that sketches are absorbed into parts while Matt Lombard worries about the ability of ST to solve all the relations in parts simultaneously. He says SolidWorks does something similar by solving all sketch relations simultaneously as well as assembly mates; these are the least reliable areas of SolidWorks in his opinion. D-Cubed is the Siemens subsidiary that provides the necessary code to SolidWorks, among others, and provides the ST code for Solid Edge and NX.
“D-Cubed proves that simultaneous solutions are not an incredibly reliable source,” he feels, and wonders if this is the reason other major CAD vendors haven’t implemented simultaneous solutions.
Future Plans
While synchronous technology may not be perfect, remember this is just Version 1; Siemens will improve on it in the years to come through continuing R&D work and feedback from users.
Paul Brown, director of NX marketing at Siemens PLM Software, says it’s ramping up investment in ST. While this release mainly targets machine designers, he says ST will be added next to the sheet-metal module and then to assembly tools. Down the road, he says the company also plans to expand ST to frames, automotive components, routed systems, pipes, flexible components and more. In addition, more Live Rules are planned, as are more geometric conditions.
In the meantime, other CAD vendors will be watching to see if synchronous technology is a Wizard of Oz concept or the Pro/ENGINEER revolution all over again. One hint in telling if it’s the Next Big Thing: look to see if Autodesk and SolidWorks announce similar-sounding technology. That may prove to be a tad tough, however, given Siemens says they’ve patented it to the hilt and do not intend to license it—for now.
Which ever way the verdict goes, the introduction of synchronous technology doesn’t mark the end for history-based modeling, for it still meets the needs of specific kinds of models—just as there is still a huge demand for 2D drafting. Instead, think of it as a third way of 3D modeling.