In a part document, you can suppress any feature.
In an assembly document, you can suppress features that belong to the assembly. These include mates, assembly feature holes and cuts, and component patterns. Sketches and reference geometry may also belong to an assembly. You cannot control the suppression of a feature that belongs to an individual assembly component.
Manual Method
To suppress individual features in the Feature Properties dialog box:
Right-click the feature 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 feature and select Configure Feature to configure the suppression state of the feature in the Modify Configurations dialog box.
Design Table
The column header for controlling feature suppression uses this syntax:
$STATE@feature_name
For example, the column labeled $STATE@Hole1 controls the suppression of the first hole.
The column header is not case sensitive.
In the table body cells, type the value for the desired suppression: Suppressed (or S, or 1), Unsuppressed (or U or 0). If a cell is left blank, the default is Unsuppressed.
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Older Method
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The following syntax was used in SOLIDWORKS 98 and earlier versions, and is included for backward compatibility: Type only the feature name in the column header cell. To suppress the feature, leave the table body cell blank. To include the feature, type any string in the body cell.
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