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 can also control the dimensions of a component contained in the assembly (by manual method only).
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
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.
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,
. Select Dimension, Controlled by Design Table in System colors and change the color.
Example of a design table that controls feature dimensions: