In either history or history-free mode, you can select a compete set of features regardless of whether they are parametric features or order-independent local features created in history-free mode. You use the Feature Faces selection type from the selection tool bar and select a face from the object or element you want to edit, and all faces related to that feature will be selected.
Figure 2: Synchronous modeling lets you easily copy, paste, and move objects.
History-free mode is an environment where linear history is not accumulated and there are no features to replay.
When working in history-free mode, you can:
In history–free mode, it’s important to remember that the Part Navigator has no timestamp order and expressions are created for commands that produce local features. There is no feature update or playback available (because there is no history), there is no rollback available (although Undo is available), and an assembly can include parts with and without history.
While this time around, synchronous operations are relegated primarily to faces, one of the more interesting objects that I modeled and modified in history-free-only mode in NX 6 was an adaptive shell. A shell consists of a wall thickness value and a collection of shell relations between its selected shell faces and partner faces (the offset counterpart of each of the shell faces in a shelled body). Shell relations in an adaptive shell can maintain the wall thickness of the shell when changes are made to it. For example, if you move a face in a shell body with the Move Face command, the shell partner face automatically updates to maintain the shell’s thickness. You can also remove all shell relations in an adaptive shell by deleting or modifying a partner face using other Face commands, such as Move, Delete, or Shell. Modifying a shell showed me that even this relatively simple change required no design interrogation that would usually be required with most other history-based modelers.
Face selection has been enhanced in NX 6, and new capabilities have been introduced with synchronous modeling that increase the potential of synchronous technology, and include Face Finder, Feature Finder, and Active Selection.
Feature and Face Finder are capabilities that seek and designate additional features or faces to copy, move, delete, etc. depending on how their geometry compares to a selected face – actually a relatively high degree of feature recognition.
Face Finder is new to NX 6 and is the logic component of synchronous technology. Face Finder searches, finds, and selects faces by recognizing geometric conditions between an input face and a set of scope faces within the model. For example, two cylinders might be oriented and located along the same axis – a coaxial condition. With Face Finder you can select one of the cylinders and recognize the other as coaxial. The Face Finder interface is available in several synchronous modeling Commands, such as Move Face (see Figure 3).
Figure 3: The synchronous modeling Face Finder and Move Face Command. When selecting the cylinder and using the Face Finder Coaxial, NX automatically selects all the geometry meeting the criteria. You then select a vector direction and drag the geometry to where you want it. Meanwhile you can see how the blends from the base of the rib updates, traversing the new surface boundaries of the cylinder.
Feature Finder was introduced in NX 5 and is enhanced in NX 6. Feature Finder is used to select an edge-connected chain of faces where the face set topologically represents an interesting feature. This is not the same as the set of faces produced when adding a NX feature, such as an extrude feature. Rather, the feature is derived by finding faces that fit a topological description. The features (topological descriptions) that are recognized by NX include boss or pocket, rib, slot, and connected blend faces.
Active selection is new to NX 6. Active selection improves selection intent. Within the synchronous modeling command set the selection intent rule defaults to “Single Face” since modifying a single face is what you’ll be doing a majority of the time.
Different Approaches With Assemblies
For many MCAD packages, large assembly performance is what sets them apart from the competition. In the previous release, NX 5, significant architectural enhancements were the basis for major improvements in large assembly modeling. To further improve assembly performance, Siemens JT data format was also integrated into NX 5. JT simplifies the pervasive multi-CAD environment that most manufacturers now deal with, as well as offering lightweight assembly design functions for faceted assembly representations that improve performance when precise solid geometry is not required, such as design reviews. To a large extent, it is the JT format that improves NX’s large assembly capacity and performance, while reducing memory usage and rendering time.
In NX, assembly part files point to geometry and features in the subordinate parts rather than creating duplicate copies of those objects at each level in the assembly. This technique not only minimizes the size of assembly parts files, but also provides high levels of associativity. This enables a user to modify the geometry of one component so that all assemblies that use that component to automatically reflect the change. These relationships not only affect assemblies, but also other associated objects, such as drawings, tool paths, and CAE meshes.
There are different approaches to assembly modeling and with NX you are not limited to any one method. You can create individual part models, and then add them to assemblies later (bottom-up), or you can create parts directly at the assembly level (top-down assembly creation). Additionally, you can start by using a top-down method, and then switch back and forth between bottom-up and top-down modeling, depending on your specific needs. It is this versatile approach that helps NX fit into a wide variety of workflows.
To assist assembly design, multiple parts can be loaded simultaneously. Load options in the NX Assembly Navigator load implicitly or explicitly as a result of being used by some other loaded subassembly. The Assembly Navigator also lets you display information and manipulate the assembly for selecting, hiding, or suppressing assembly components. Additionally, loaded parts do not have to belong to the same assembly. The part currently displayed in the graphics window is called the displayed part. You can make edits in parallel to several parts by switching the displayed part back and forth among those parts.
An assembly can contain a mixture of parts modeled with history or history-free mode. This is not actually new. Even prior to the NX 6 this combination could be used. If you import a Parasolid .x_t (or other) part into a NX part file it has no history. This part can coexist in a NX assembly with native NX parts complete with features and history. Also, an assembly can contain a mix of parts and JT files, so if you are working with a supplier or OEM who provides only lightweight data for building an assembly, you can reference JT data and build models that are the correct size and shape.
When the displayed part is an assembly, you can change the work part to any of the components within that assembly (except for unloaded parts and parts of different units). Geometry, features, and components can then be added to or edited within the work part. Geometry outside of the work part can be referenced in many modeling operations. For example, control points on geometry outside of the work part can be used to position a feature within the work part. When an object is designed in context, it is added to the reference set used to represent the work part