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Siemens PLM Software’s Solid Edge Gains Efficiency from Synchronous Technology

By Al Dean

This image illustrates a face being pulled up and a value dialed in.Figure 1: This image illustrates a face being pulled up and a value dialed in. Note that planar faces are also adjusted (these, of course, can be overridden, so the system doesn’t get too carried away). Also worth noting is that the system maintains the fillet/blend as well as the draft angle that’s applied to the outside of the part.

In May of this year, Siemens PLM Software unveiled the future of its 3D modeling strategy with the launch of Synchronous Technology. This represented — many claimed — the next big thing, a breakthrough for modeling tools, and would result in Siemens PLM’s MCAD offerings being catapulted ahead of the rest of the pack.

But what is it? And what does it mean, in the scope of this review, for Solid Edge? To answer that, we need to understand what Synchronous Technology is and then to look at how it is being implemented within Siemens PLM’s mainstream offering, Solid Edge. And to get there, we must first look at how Solid Edge currently works.

Solid Edge is a feature- and history-based modeling system, meaning each modeling operation is stored within a history tree. When edits are made, the system needs to re-calculate each one after the other, to arrive at the final form. Within that, the system also includes parametric design tools, allowing dimensions, constraints, and other driven parameters to control the form of entities within each feature and to cross-link between them.

Parameters range from dimension and geometric constraints within a feature sketch to parameters that define feature extents (such as extrude height and cut depth). You can set up parameters or constraints that link between features and geometry references, using, for example, the “extrude to” option, or offset. Then you can also build parameters that are intelligently driven, referencing other dimensions or measurements.

Here, the system works with concentricity and tangency.
Figure 2: Here, the system works with concentricity and tangency. You select the hole, use the onscreen widget to move it precisely, and because you also have a concentric condition, the whole bracket stretches. The outer edge maintains its concentricity and the tangency of the swing arm is maintained.

These are the core components of any Solid Edge model — Features, History, Parameters, and Constraints. To confuse things further, you also have a few direct editing tools that allow localized modifications to faces (such as Move Face) without having to edit the base feature. These are appended to the end of the history tree and should also be considered to be features (with history). Synchronous Technology changes this state of affairs: Siemens PLM has taken its Parasolid and D-cubed technology and created a layer on top to extend them. This is the essence of Synchronous Technology and it allows you to work in a more efficient manner than has traditionally been the case with Solid Edge.

Synchronous Technology is a feature-based, yet history-free modeling technology. In other words, it allows you to work with features, enhances the current tools by freeing you from the need to recalculate the history after each edit, and adds intelligence to your working process.

Let’s dig a little deeper and look at two specific cases: the first, when modeling from scratch and, perhaps more critically to existing users, how you use Synchronous Technology with your existing data.

Modeling from Scratch
Synchronous Technology (ST) enables users to create parts in a freeform manner. You sketch, then use a set of commands to create the geometry. ST is currently enabled in a select set of operations, but the selection of Extrude, Revolve, Hole, Round, Draft, Pattern, and Thin Wall (or Shell) is a little deceptive. You need to consider that each enables both the cutting and addition of material in a single feature, and the manner in which you interact and manipulate geometry means that you have more potential in terms of forms that can be created.

By selecting the boss and the end face of a model using Synchronous Technology, you can stretch the part as you need to, rather than having to dive in and edit several features right back to the original extrude that created the pipe.
Figure 3: By selecting the boss and the end face of a model using Synchronous Technology, you can stretch the part as you need to, rather than having to dive in and edit several features right back to the original extrude that created the pipe. What’s absolutely key to note is that at no point are you editing features in a history—you make your edits and the system updates automatically.

So, you create a sketch, and the direction in which you drag the arrow defines whether material is added or removed. What enables the freedom is the fact that you are presented with a great deal of feedback. If you grab a face and move it, you can do it by eye or dial in a specific value (see Figure 1). It’s the same for rotation: References are created on the fly and the Steering Wheel widget is useful for moving and rotating geometry in 3D space. Also, when you drag and drop faces, the system works with a set of selection assistants that add intelligence to the process. These are called Live Rules and infer relationships such as tangency, parallelism, concentricity, perpendicularity, symmetry (around a define plane), and radii, between the geometry you select and the geometry that exists around it as seen in Figure 2.

But while it’s interesting to play with geometry to get a model into shape, within the design world you always need to be able to tie up specific dimensions and controlling factors — and this is what makes Synchronous Technology unique (for the time being at least). At any point, you can add dimensions or constraints, which can have specific values. These can be between faces, edges, and other geometric features, they can be driven or driving, be linked using parametric equations, and can reference each other. The point is that you apply them only when they’re needed and they are then maintained. The result is that your interaction with the geometry will respect those constraints, and dimensions are maintained — and again, all without having to resolve a history tree with each edit.

For example, Figure 3 shows a dimension between the center of a boss and the end of a fixture. As you drag those features, the dimension is maintained, because you’ve defined it. You work with assemblies in a very similar manner, in that you grab, drag and drop, move, and rotate faces in multiple parts and the system will calculate the updates automatically. In addition, references can be made between separate parts, cross-referencing faces where required.

Working with Existing Data
While ST is an interesting modeling technology, how does it affect your existing data? Some organizations have been using Solid Edge for more than 10 years and have built up a huge amount of live data, but how can they adopt this new way of working and still maintain that data? The answer is simple — leave it as is. Solid Edge is now architected to work in two modes: the standard way, with the full range of features and functions that have made it a most impressive application, and also with ST enabled. But you need to be aware of some things.

Dimensions have been placed after the design work has been done, in order to formalize the design intent and lock down dimensions.
Figure 4: Dimensions have been placed after the design work has been done, in order to formalize the design intent and lock down dimensions. What’s key is that you can also create the same parametric relationships between dimensions to drive design changes as you would within a history and parametric modeling system. Here, a hole feature is maintained froma traditional Solid Edge component—all of the design intent (in terms of bore size, thread information) is retained and editable.

When you open a new part, you have two options. You can either open the part with the traditional feature- and history-based modeling tools or you can use an ST-enabled template, which activates these new tools. More importantly though, if you take a traditional history-based model with a rich history of features that control its design and open it in ST mode, the system prunes out the history, but retains the information required to maintain the features in a Feature Collection.

Siemens refers to these features as Procedural Features and they include things like chamfers, blends, patterns, and shells. This means you can edit them and the system will maintain the design intent you stored within them (see Figure 4). For example, even though a pattern is typically a history-based feature, you can still edit the number of holes, say, within an array or edit the dimensions of the holes using standard hole-definition terminology (such as counter sink or counter bore).

Vital Signs
It’s important to note that you can’t really take a part back into the traditional modeling environment once you’ve completed ST-based work. If you do, then the system treats it as a dumb solid. It’s also worth noting that you can put ST parts in a traditional assembly and they will update as need be. These things are key to working out an adoption strategy.

Synchronous Technology is brand new. Yes, many of the components have been around for some time, but this is the first time that you’ve been able to combine the flexibility of explicit modeling tools such as CoCreate with the parametric- and feature-based tools within Solid Edge and others. The fact that the system can solve and handle design changes with such ease means many things, but the bottom line is this: If you can affect design change within a part or assembly without having to first work out the complex history that gets you to the end result, then you’re looking at a radically more efficient product development process.

Synchronous Technology has set tongues wagging across the 3D design world. If you ‘Google’ the term you’ll find endless amounts of blogging about it to varying degrees of accuracy, and many have tried to pull it apart. What’s been missed to date is that this technology is at a formative stage in development. Yes, you can do a hell of a lot, but you don’t get all those other tools — part, assembly modeling, sheet metal, surfacing, pretty much everything — that have been a core part of Solid Edge for the last decade.

Within Solid Edge, you now have two choices — to go synchronous or not. When you do or don’t depends on your projects and even individual parts. The benefit is that the ST-enabled tools make light work of modeling, and when they can’t create what you need, you have the last decade’s worth of Solid Edge technology available to do things the traditional way. Just make sure you are aware of its limitations and understand the impact of moving existing data.

The good news remains that this technology has huge potential and, even at this early stage, it’s clear that Siemens has something unique on its hands. 

More Info:
Siemens PLM Software
Plano, TX


Contributing Editor Al Dean is the editor at DEVELOP3D, a new UK product development and manufacturing technology journal. He divides his time between day dreaming about owning a 5-axis NC machine and having nightmares explaining its purchase to his family. Send comments about this article to DE-Editors@deskeng.com.

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DE's editors contribute news and new product announcements to Desktop Engineering. Press releases can be sent to them via DE-Editors@deskeng.com.