In a part document, you can suppress any sketch.
In an assembly document, you can suppress sketches created in the assembly. You cannot control the suppression of a sketch created in an individual assembly component.
Manual Method
To suppress individual sketches in the Feature Properties dialog box:
Right-click the sketch you want to suppress in the FeatureManager design tree and select Feature Properties.
In the dialog box, select Suppressed, and then
select This Configuration, All Configurations, or Specify Configuration(s).
You can also right-click a sketch and select Configure Feature to configure the suppression state of the sketch in the Modify Configurations dialog box.
Design Table
The column header for controlling sketch suppression uses this syntax:
$STATE@sketch_name
For example, the column labeled $STATE@Sketch1 controls the suppression of the first sketch.
The column header is not case sensitive.
In the table body cells, type the value for the desired suppression: Suppressed (or S), Unsuppressed (or U). If a cell is left blank, the default is Unsuppressed.