January 26, 2009
NX 6 – Synchronous Modeling Promotes Design Freedom
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In NX all drafting objects are associative. Some drafting objects, like dimensions, are linked directly to geometry so that they automatically update when changes occur. Other drafting objects, such as notes, are associated to a position rather than specific geometry. Some drafting objects, such as labels, ID symbols, forms and positional tolerances, can be associated to either the geometry or to a position.
You can associate non-geometric information with objects and parts. You can link attributes to objects in order to record special characteristics of the objects.
There are two types of attributes – system and user-defined. System attributes are recognized by the system and assigned by a user, such as when you assign a name to an object or a group to aid in the selection process, the system will recognize that name until you explicitly change it. User-defined attributes are those that you create, but have no meaning to the system. For example, you may associate attribute information to a group of geometric objects so they appear correctly in the bill of material for the product.
You can position a feature 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.
Expressions let you incorporate design requirements and restrictions by defining mathematical relationships between different parts of a design. For example, you can define the height of a boss as three times its diameter, so that when the diameter changes, the height also changes.
Other NX applications can operate directly on solid objects created within Modeling without translating the solid body. For example, you can perform drafting, engineering analysis, and NC machining functions by accessing the appropriate application. You have to remember to save changes made to your layout before entering the Drafting application. If you do not save the changes, they are gone when you return to the Modeling application.
A model can be updated either automatically or manually. Automatic updates are performed only on those features affected by an appropriate change (an edit operation or the creation of certain types of features). If you wish, you can delay the automatic update for edit operations by using the Delayed Update on Edit option.
The manual method that I liked best was the Playback option on the Edit Feature dialog that recreates the model starting at its first feature. You can step through the model as it is created one feature at a time, move forward or backward to any feature, or trigger an update that continues until a failure occurs or the model is complete. The Edit during Update dialog, which appears when you choose Playback, also includes options for analyzing and editing features of the model as it is recreated (especially useful for fixing problems that caused update failures).
Synchronous Modeling in NX 6
NX 6 has two modeling modes – history and history-free – and you can take advantage of the benefits of each – sort of a best of both worlds sort of thing. The two modeling modes and the ability to switch between them are what set NX 6 apart and constitute Design Freedom, however, Synchronous Technology works in either of the modeling modes. Because you can use both modes in NX 6, you might find that the history-free mode is well-suited for the conceptual stage of a design and the history mode well-suited for the refinement stages of a design.
In history mode, you create and edit models using an ordered sequence of features that are displayed in the Part Navigator. This mode is most useful for parts that are highly engineered.lIt is also useful for parts that will be modified using predefined parameters based on the design intent built in to their sketches, features, and feature order used to model the parts.
In history-free mode, you create and edit models based on their current state without an ordered sequence of features – only local features without a sequential structure are created. Local features are unique because they are created and stored in history-free mode. Modifying a local feature affects only the local geometry without the need to update and replay a global feature tree. This is one of the primary reasons that local features can be edited much quicker than features in history mode. Synchronous modeling is also what lets you create geometry that adapts to a changing design context.
The Synchronous Modeling toolbar is your main ally for synchronous modeling and consists of the following commands that will provide you with a better understanding of what it can do (see Figure 1):
Note: All of the commands except Shell body and Cross Section Edit are available in both history and history-free modes.
Figure 1: The Synchronous Modeling Toolbar
In NX 6 you can change the design mode between history and history-free, however, due to the differences between the two modes data unique to each mode is removed when the mode is changed. For example, when changing from history mode to history-free mode history data is deleted, including feature data. Geometry remains in its current state but features are removed, similar to using the Remove Parameters command. However, features that are local features are retained, so features such as holes and blends remain as holes belnds, but become local features.
When history-free mode is set, history-related commands are hidden in the interface. For example, Edit with Rollback, Reorder Feature, and Replay are hidden.
Specific synchronous modeling commands are used to modify a model, regardless of its origins, associativity, or feature history. A model can be imported from other CAD systems, neutral formats (IGES and STEP), non-associative, with no features, or it could be a native NX or Solid edge model with features. Synchronous modeling lets you use parametric features without the problems arising from feature history by working directly with a model that virtually eliminates time spent rebuilding or converting geometry. In short, if you have a parametric model that you want to edit quickly, use synchronous techniques in history mode.
I found that synchronous modeling is best suited for models composed of analytic faces, such as plane, cylinder, cone, sphere, and torus. This does not necessarily mean simple, geometrically primitive parts, since models with literally thousands of faces can be composed of these analytic face types. A deficiency that I noted in NX 6 is that synchronous modeling does not work well with blends that would be found in cast or molded parts, but the company is working on this for future release.
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-- Jeff Rowe, MCADCafe.com Contributing Editor.