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Part Navigator Dependency Pane in NX 11.0.1

Siemens Phenom Siemens Phenom
Siemens Phenom

Browsing dependencies in the part navigator is now easier in NX 11.0.1. For this reason, I thought it would be good to explore some commonly misunderstood details of this aspect of the part navigator.   

The dependency browser shows the relations for the selected object. This object can be a piece of geometry, a feature, or even an assembly constraint. Please note that selecting a solid body is not the same as selecting an extrude feature. NX might highlight the same object in the graphics window, but they are not the same. NX has a dual nature where there is a difference between selecting a display object (something that you can show and hide or put on a layer) and a feature.

In the navigator, features are shown with a green check (suppress check) and objects are shown with a red check (visibility check).

In ancient days, the part navigator was strict and forced you to select an object in order to be able to hide it; features could not be hidden. Luckily for all of us, those days are passed and you can now select an extrude feature to hide. NX hides the geometry that is produced by the feature. But it does help when you understand that there are two concepts of objects in NX. You can create an extrude that produces two bodies and then “put the extrude feature on layer two.” You should understand though that that is not really true. You can select one of these bodies and put it on layer three. On which layer is the extrude feature now?

PN1.jpgNew folder at the top of the navigator

In NX 11.0.1, a new Non-timestamp Geometry folder in the part navigator makes it easier to find the objects that are not produced by any feature. These non-timestamp objects now also participate in the dependency browsing.

Now that you understand the importance of distinguishing between objects and features, you should find the dependency pane in the navigator easier to use.

When you select a feature, such as the extrude in the picture below, the dependencies of the feature are then shown in the dependency pane. The Children folder contains all features that directly depend on the selected feature. The Parents folder contains the features and objects on which the selected feature directly depends.

PN2.jpgDependencies of an extrude feature

Here you can see that a line object was referenced in the extrude feature.

By default, the Detailed View toggle is OFF, which means we are looking at the feature. When you change the Detailed View toggle to ON, the dependency browser allows you to look inside of the feature.

The inside of the feature reveals the detailed inputs. The Children folder shows the objects that are produced by the feature, including those objects that are referenced by other features. In the example here, the solid is the output of the extrude. 
The edge is blended downstream and the face is moved by a move face feature. This extra information could be useful when you plan to replace the feature with another. It provides a clue as to how many objects will have to be mapped.

The Parent folder shows how the feature works. You can even see the selection intent rules that were used to define the section. You can also see that the extrude direction was inferred from the sketch object (red check!).

PN3.jpgFeature recipe shown in the dependencies pane

In NX 11.0.1, when you select the XY datum plane of the datum CSYS through QuickPick, you will see that the information on the objects of the datum coordinate system feature is much improved. You can now see which plane of what feature you are selecting. This of course also helps when browsing dependencies.
PN4.jpgObject names and feature names

In this case, I named the datum CSYS feature (feature name) and the XY plane of the datum CSYS (object name) through properties. The feedback now shows all the names of the selected object, while still indicating it is the XY Plane of a datum coordinate system.