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Base Parts in Configurations
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Component Suppression State in Configurations
Cosmetic Threads in Configurations
Derived Configurations in Design Tables
Description in Configurations
Dimensions in Configurations
Display States in Configurations
End Conditions in Configurations
Expand in BOM in Configurations
External Sketch Relations in Configurations
Feature Suppression State in Configurations
Shortcuts for Suppressing Items in Design Tables
Fixed or Floating Position in Configurations
Global Variables in Configurations
Hole Sizes in Configurations
Lighting in Configurations
Mass Properties in Configurations
Materials in Configurations
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Sketch Suppression State in Configurations
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Glossary
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Feature Suppression State in Configurations

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.

Older Method

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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