Dimensions in Configurations
You can apply dimension values to selected configurations as follows:
In a part
document, you can control the dimensions in sketches and in feature definitions.
In an assembly
document, you can control dimensions that belong to assembly features.
This includes mates (angle or distance), assembly feature cuts and holes,
and component patterns (spacing or instance count). You cannot control
the dimensions of a component contained in the assembly.
To manually modify a dimension
value for a selected configuration:
Double-click
the feature to display the dimension.
Double-click
the dimension, change the value in the Modify box, and select one of the
following (these options are only available if there is more than one
configuration in the model):
You can also right-click
a dimension and select Configure
dimension to configure the dimension.
You can also control dimensions
in a design
table.
The column header in a design
table for controlling dimensions uses this syntax:
Dimension@Feature
or Dimension@Sketch<n>
For example, the full name for the depth of an extrude feature is D1@Extrude1; the full name for the
dimension of the first Distance
mate is D1@Distance1. You can
assign meaningful names to dimensions in the Dimension
PropertyManager, under Primary Value.
The column header
is not
case sensitive.
In the table body cells, type the value for the dimension. If a cell
is left blank, it inherits the current dimension at the time the configuration
is created.
NOTES:
When you
specify values, be sure to use the system of units specified for the model
document (click Tools, Options,
Document Properties, Units).
You can
display dimensions that are driven by design tables in a different color.
Click Tools, Options,
System Options, Colors. Select Dimension, Controlled by Design Table
in System colors and change the
color.
Example of a design table that controls feature dimensions:
![](../art_local/design_table_feature_dimension.gif)