Part Modeling > Sections in Sketch-based Features > About Sections in Sketch-based Features
About Sections in Sketch-based Features
Sketch-based features use a Sketch feature (a sketch) to define their shape, dimensions, and general placement. You use a Sketch feature to create sketch-based features in the following ways:
Create an internal section—You can create an internal section (also known as a section) while the sketch-based feature tool is open. You use Sketcher to create the sketch, thus defining the internal section. This internal section is independent and is not associative with any Sketch features. So, the changes that you make to an independent internal section affect only the sketch-based feature using that internal section. This independence is further indicated by a unique name that is assigned to each independent internal section.
Select a Sketch feature—You can select an existing Sketch feature (sketch) to create a sketch-based feature. The Sketch feature can reside in the current model or in a different model. You can also use a Sketch feature that has already been used as a reference for a different sketch-based feature.
* Sketched point features created before Pro/ENGINEER Wildfire 5.0 are converted to sketch features containing geometry points.
After you create a sketch-based feature by selecting a Sketch feature, Creo uses the Sketch feature placement, orientation, and sketch references to create a dependent internal section for the sketch-based feature. This dependent internal section is fully associative with the parent (referenced) Sketch feature. It also shares its name with the parent. So, if you redefine the parent Sketch feature, all dependent internal sections (children) that reference this Sketch feature will dynamically change. This changes the respective sketch-based features. Conversely, if you redefine a dependent internal section, Creo automatically rolls back to the parent Sketch feature enabling you to redefine it.
Valid and Invalid Sections
Sketch-based features may have requirements such as a closed loop section (sketch), a vertical axis, or a coordinate system. The system tracks these feature-specific requirements against the section that you are using. If the section does not satisfy these requirements, The system does one of the following:
If you are creating an independent section, the system warns you that the section is invalid.
If you are creating a dependent section by attempting to select an invalid Sketch feature, the selection filters will prohibit the Sketch feature from being selected.
If you delete a parent Sketch feature (one that is being used as a reference for a dependent section), the system displays a warning and provides options for you to resolve the broken parent-child relationships resulting from deleting a parent feature.
You can use sketch-based features from previous Pro/ENGINEER releases. However, if an older sketch-based feature cannot be fully referenced, the Section Selection dialog box opens warning you that Use Edge technology will be used to acquire the necessary sketch geometry for the internal section.
Although you can create a Sketch feature that consists of only construction entities and one or more geometry centerlines, this type of section cannot be used to define a sketch-based feature.