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:
$TOLERANCE@Dimension
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:
![](../art_local/design_table_tolerance.gif)