||This task shows you how to create dimensions that will
drive associated geometry.
You can create the following types of driving
- distance (and distance offset in the case of two concentric circles)
||Go to Tools > Options > Mechanical Design > Drafting >
Dimension and select Activate analysis display mode. Then,
click the Types and colors button. The Types and colors dialog
box is displayed.
Make sure the Dimensions driving 2D geometry
check box is selected, and identify the color that will be assigned to
driving dimensions (you can change it if you want).
Create a line. Click the Dimensions
icon from the Dimensioning toolbar and
create a length dimension on this line.
Double-click the dimension. The Dimension value dialog box is displayed.
Make sure the Drive geometry check box is
selected. This dimension will now drive the geometry.
Modify the dimension value, entering 40 millimeter as the
Click OK to validate and exit the dialog box.
The geometry is updated according to the new driving dimension value.
Click elsewhere in the drawing to deselect the dimension.
You can see that the driving dimension is assigned the colors defined in
the Types and colors dialog box.
||You cannot create driving dimensions between the following types of
elements (in this case, the Drive geometry option is deactivated
when double-clicking the dimension):
- Once the Drive geometry check box is selected, you can
access a contextual menu and customize the values properties according to
your needs. For more information on the available options, refer to CATIA
Knowledgeware Infrastructure - Tips and Techniques - Summary, available
from the Using Knowledgeware Capabilities section in the
Infrastructure User's Guide.
- When a driving dimension is created between two parallel lines, then
their parallelism is constrained. Therefore, if a geometrical parallelism
constraint was previously applied to them, this constraint is destroyed.
This avoids an overconstrained situation.