Part Modeling > Base Features > Extrude > Basics of the Extrude Feature > About Sections Used for Extrusions
About Sections Used for Extrusions
You must define a section to extrude. Use one of the following methods:
Click Model > Extrude and then sketch a section. To create a section, click the Placement tab, and then click Define.
Select a sketch before clicking Model > Extrude.
While the Extrude tab is open, create a sketch to use as a section. To create a sketch, click Model > Sketch.
Activate the Extrude tool and select a sketched datum curve.
Sections for Solid Extrusions
These rules apply to solid extrusions, and do not apply to cuts, thickened features, and surfaces.
Extruded sections can be open or closed.
Open sections can have only one contour. All open ends must be aligned to the part edges.
Closed sections may consist of the following:
Single or multiple closed loops that do not overlap.
Nested loops, where the largest loop is used as an outside loop and each other loop is considered to be a hole in the larger loop. The loops cannot intersect each other.
Sections for Cuts and Thickened Extrusions
These rules apply to cuts and thickened extrusions:
Sections can be open or closed.
You can use an open section with ends that are not aligned.
A section cannot have intersecting entities.
Sections for Surfaces
These rules apply to surfaces:
You can use an open or closed section.
A section can have intersecting entities.
Using Sections with Multiple Contours
When you add an extrusion to existing geometry in a part, you can sketch several contours on the same sketching plane. These contours cannot overlap, but they can be nested. All extruded contours share the same depth option and are always selected together.
You can also sketch multiple loops within the section outline to create voids (islands) inside a protrusion.