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Tolerances in Configurations

In the Dimension PropertyManager, when you specify a tolerance, you can assign it to This configuration, All configurations, or Specify configurations.

In a design table, you can control tolerances as follows:

  • In a part document, you can control the tolerances on dimensions in sketches and in feature definitions.

  • In an assembly document, you can control the tolerances on dimensions that belong to assembly features. This includes mates (angle or distance), assembly feature cuts and holes, and component pattern spacing. You cannot control the tolerances on dimensions of a component contained in the assembly.

The column header in a design table for controlling tolerances uses this syntax:


For example, the tolerance on the depth of an extrude feature is $TOLERANCE@D1@Extrude1; the tolerance on a distance mate is $TOLERANCE@D1@Distance1.

The column header is not case sensitive.

In the table body cells, type the value for the tolerance, using a valid keyword and syntax. If a cell is left blank, the dimension has no tolerance. For a derived configuration, if a cell is left blank, the component uses the tolerance value of its parent.

When you specify values, be sure to use the system of units specified for the model in Units Options.

Example of a design table that controls a tolerance:


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