||Up to Part Design Version 5 release 14 the
sketches used for creating sketch-based features were located directly
below the features in the specification tree. Now, to improve the
visibility of your design process this behavior has changed: depending on
how sketches are created, sketch entities are not necessarily displayed
below the features they support.
This page covers the following topics:
Entities Aggregated by Sketch-based Features
The sketches used for creating
sketch-based features are aggregated by, or to put it in another way,
located just below those features in the tree when:
You are working in a
hybrid design environment.
You are using a sketch created
prior to the feature
The sketch is not already
aggregated by another feature
Sketch Entities Referenced by Sketch-based
- Sketches are referenced by sketch-based features when these sketches
are already aggregated by previous features. In the example below, Pad.4
references Sketch.6 which is already use to create Pad.3.
- Sketches are referenced by sketch-based features if these sketches
are not directly located above the node of the features you are creating.
In the example below, Pad 4 created using Sketch.7 because an
intermediary feature, Draft.1 was created after the sketch.
Specific Cases: Ribs, Slots, Multi-section
Solids and Solid Combines
Ribs, slots, multi-section solids and solid combines require the use of
two sketches at least.
- If these sketches are successively located in the specification tree,
Specific Cases: Power Copies and User Features
When selecting a sketch-based feature to define a
Power copy or a
User Feature, remember that:
- if the sketch is aggregated (placed just below the feature in the
specification tree), that sketch is included in the selection as shown
under Inputs of components.
- otherwise, if the sketch is referenced, it is not therefore included
in the definition of the power copy or user feature. If you need to
include it because it will be requested at instantiation, do select it.
Reordering Sketch Locations
The rules mentioned above apply when you are creating sketch-based
features. But when you are editing those features, at any time, you can
modify the location of a sketch by using the Reorder capability.
This capability moves and repositions sketches at the location of your
choice, provided that the location you choose does not affect the integrity
of your part. The application provides a quick help for that. For more
information, refer to
Reordering Features and
Reordering Sketch-Based Features.