Part Modeling > Sections in Sketch-based Features > Using a Sketch as a Feature Section
Using a Sketch as a Feature Section
You can use an existing sketch as a section for sketch-based features. The default feature type depends on the selected geometry:
If you select an open sketch, the tool by default creates a surface.
If you select a closed sketch, the tool by default creates a solid protrusion. You can later change solid geometry to surface geometry.
* In Assembly mode, the default feature type is solid cut.
Consider the following rules on using an existing sketch as a feature section:
You cannot select a copied sketch.
If more than one valid sketch was selected or if the selected geometry was invalid, the tool opens with no geometry collected. The system displays an error message and asks you to select new references.
Associativity between the Selected Sketch and the Feature
By default, when you select a sketch to use as a feature section, the section becomes associative with the original sketch. You can break this associativity and make the sketch independent by clicking the Placement tab, and then clicking Unlink. When you unlink the section, the sketch is copied into the feature and becomes and an internal sketch.
The Model Tree reflects whether the sketch used is internal or external. If you selected a sketch to use as the feature section, clicking the feature node shows the node for the sketch. If you redefine the feature and unlink the sketch, its node under the feature node changes to that of an internal sketch.
If you created a sketch while in the tool, a group is created that includes the sketch and the feature.