Sketch environment

The sketch environment consists of a sketch plane (where the sketch is located) and sketch commands to create, edit, constrain, and dimension geometry. When you click the Sketch tab, the sketch environment becomes active.

You close the sketch environment when:

• In a part file, you select a sketched feature command (extrude, revolve, sweep, loft, or coil) from the Model tab. The feature you create uses the sketch as a profile or path .
• In an assembly file, click the Create command from the Assemble tab. You also close the sketch environment when you activate a component or the top-level assembly.
• In a drawing file, you select a drawing command from the Drawing panel bar.

You click Finish Sketch on the ribbon to end a sketch . The sketch is designated in the browser by a sketch icon. Sketches that have been consumed by features are listed in the browser under the feature icon.

When the sketch command is selected, you can choose a planar face , work plane , or sketch curve to specify the sketch plane. Selecting curves from a previously created sketch reopens that sketch so that you can add, modify, or delete geometry. Selecting a face redisplays the feature sketch for editing.

Finishing the first sketch in a new part file takes you automatically to the Home (isometric) view. This greatly facilitates the viewing and creation of extruded and/or revolved features using Direct Manipulation operations.

Each time you finish a sketch, a sketch icon is placed in the browser. For example, if you click the Sketch command, select a part face, and then click the command again to close the sketch, a sketch icon is placed in the browser even though you did not create any geometry.

When you create a sketch in an assembly, the sketch icon is nested under the Origin folder of the top-level assembly in the browser. A sketch icon for a sketch created in a part included in an assembly is nested under the part icon in the browser.

A sketch is associated with a face or plane even if you created no geometry. A part face used as a sketch plane has sketch boundaries represented by the bounding edges of the part face. A work plane has no boundaries and represents an infinite sketch plane, though it is associated with the geometry used to create it.

You can select the sketch icon and edit the sketch with new geometry, constraints, and dimensions.

Use any of the following methods to create a sketch:

• Start a new part file. By default, a sketch is created and active.
• Click a planar face or work plane of another part in an assembly.
• Drag off of a planar face or work plane of another part in an assembly.
• Start a new assembly file. Expand the Origin folder and make an origin work plane visible, and then select it as the sketch plane.
• In an assembly, click a planar face or work plane.