January 26, 2009
NX 6 – Synchronous Modeling Promotes Design Freedom
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As a long-time product designer I’ve been a member of the CAD community since the late 1980s and have followed developments (good and bad) closely since then. In the early days, it seemed like just about every release of software contained a bunch of new features and capabilities – some useful, some not so useful. “Feature bloat” became a real problem with a lot of MCAD products at the expense of real utility and stability. Recently, however, most MCAD vendors have become more concerned with product quality and reliability than just continuing to pile on more “stuff,” that few customers understand or actually use.
In the spring of 2008 Siemens PLM Software announced not just a new feature or capability set, but a new CAD methodology that it claimed to be the biggest MCAD breakthrough in a decade called Synchronous Technology. At the time, the announcement was actually more speculative than a true demonstration, but nonetheless, from the beginning, the concept and its implications were pretty intriguing. Synchronous Technology that forms the basis for synchronous modeling were integrated into the newest versions of Siemens’ MCAD products – NX 6 and Solid Edge ST. Using NX and Solid Edge as vehicles, Siemens PLM Software became the latest MCAD company to tout the advantages of
non-history-based design methods. However, NX 6 has a notable difference with the way synchronous technology is implemented in what the company calls Design Freedom that I’ll discuss later. Also, NX 6 differentiates itself with the fact that synchronous technology can be used in both history and history-free modes.
Before we jump into synchronous technology and synchronous modeling, I think it’s worthwhile to briefly cover the three underlying technologies that form the basis for the geometry component of synchronous technology and synchronous modeling:
Siemens PLM Software collectively refers to these core geometry technologies as its “geometry triangle.”
The “change” technology is used to modify the faces of a model. This technology is the basis for several synchronous modeling commands, such Move Face, Offset Region, Resize Face, and Make Coplanar. Within the Move Face command the change technology moves selected faces and adapts neighboring faces to accommodate the change.
The “delete” technology is employed to remove faces from a model. This technology is the foundation of the Delete Face and Cut Face commands. The delete technology deletes selected faces and heals neighboring faces to close the open area left where faces are deleted. Delete has enhanced support for merged faces and dependent blends.
The healing function is the emphasis for delete technology. Limitations are being addressed but there will be cases where neighbor faces cannot heal an open area. In this case you can incrementally delete smaller sets of faces with multiple uses of the Delete Face command. The Replace Face command can also serve as alternative to Delete Face.
The “re-blend” technology is a companion to “change.” It is employed to adapt blend faces when selected faces change (move and offset), and also applies to constant radius rolling-ball blends.
So, with this little bit of background, let’s take a look at what NX 6 is about and what it can do.
Getting Started With NX 6
For the purposes of this review, I received the core NX 6 application pre-loaded and configured on an HP Compaq nw9440 mobile workstation. It had an Intel Core 2 CPU running at 2.16 GHz, 4GB RAM, nVIDIA Quadro FX 1500M video card, and Microsoft Windows XP Pro SP2. This set up was more than adequate for the part and assembly solids and surfaces that I modeled with NX 6 (188.8.131.52).
It wasn’t all that long ago that NX’s interface was known as being quite intimidating. However, with NX 5, a lot of that changed as the UI became much more Windows-compliant, and, therefore, more user friendly. A big part of the movement toward ease of use are NX’s Roles that let you customize and limit the UI by hiding tools that you are unlikely to use. This is especially important to new NX users, or so-called casual users who can use the default Essentials role. In this default role, the command buttons display both icons and the command name. If you want a more comprehensive set of tools, click the roles tab in the resource bar and select a more advanced role. It
you have used an earlier version of NX, you can reinstate your previous UI layout from the Last Release folder in the roles palette.
The UI, roles, and customization combined are what help give NX 6 the ability to accommodate a wide variety of users and workflows.
As far as command flow is concerned, and to further illustrate how the UI continues to improve, commands are displayed in dialog boxes that are organized by workflow that let you logically work from top to bottom to perform a command. A red asterisk marks steps that require some selection, and a green check mark replaces the red asterisk after a suitable object is selected. An orange highlight indicates that the current selection is active, while a green highlight indicates the next recommended step. When all required inputs are completed, the OK or Apply buttons are highlighted in green. To keep things relatively simple, some commands, such as Dimension Creation, are optimized to
complete automatically and loop after you make the required selections, and only have a Close button.
Models, assemblies, drawings, and most other objects created in native NX 6 are saved as parts with a .prt extension, and you can open as many parts as you want or need to at any time. If you have Teamcenter integrated with NX, parts are stored as datasets and identified by part numbers. Specifically for drawings, to make things more efficient with a more direct workflow, I’d recommend that you use a “master model” approach that separates the drawing part from the model part by using a drawing template that automates this method.
Like virtually all MCAD packages, parts in NX 6 often begin with sketches as one of its several available design approaches. The sketcher is an NX tool for creating 2D geometry within a part, and each sketch is a named collection of 2D curves and points on a specified plane.
The strategy you use to create and edit your model to form the desired object depends on the form and complexity of the object. In reality, you will probably use several different methods during a design session.
NX sketcher tools let you capture design intent through geometric and dimensional relationships, collectively referred to as constraints, to create parameter-driven designs that can be updated later. Sketcher continuously evaluates constraints to ensure that they are complete and do not conflict. Sketcher also lets you create as many, or as few, constraints as required.
You use NX’s sketcher to freehand a sketch, and dimension an outline of curves. You can then transform the 2D sketch into 3D using tools such as Extrude or Revolved Body to create a solid or sheet body. You can later refine the sketch to precisely represent an object by editing the dimensions and by creating relationships between geometric entities. Editing a sketch dimension modifies the geometry of the sketch, as well as the body created from that sketch.
You can position a feature, such as a hole or groove, relative to the geometry on a model by using positioning dimensions. The feature is then associated with that geometry and will maintain those associations whenever you edit the model. You can also edit the position of the feature by changing the values of the positioning dimensions. If the model is edited later, the associated drawing and dimensions are updated automatically.
Although it can produce some outstanding surfaces, getting to a final solution can be somewhat challenging because some of the curve creation tools can take some trial and error to arrive at the precise shape and form you are looking for.
Overall, though, once you get beyond some NX nuances, creating sketches and parts is about on par with other MCAD packages – not really any easier, but definitely not as difficult as many have been mistakenly led to believe.
NX uses the concept of associativity to link separate pieces of information together that helps automate part design.
Associativity is used to indicate geometric relationships between portions of a model. Associativity is used when creating geometry. For example, an object may be part of the model (in Modeling) or specifically linked to a single view (in Drafting). These relationships are established as you create a model. In an associative model, constraints and relationships are captured automatically as the model is developed. For example, in an associative model, a through hole is associated with the faces that the hole penetrates. If the model is later changed so that one or both of those faces moves, the hole updates
automatically because it is associated with the faces.
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-- Jeff Rowe, MCADCafe.com Contributing Editor.