Using the Sub-Elements of a Sketch

This task shows you how to select different elements belonging to the same sketch for creating pads.
The steps described here also apply for pockets, shafts, grooves, stiffeners, ribs and slots.
Sketch three rectangles in a Sketcher session.
1.	Click the `Pad` icon . The Pad Definition dialog box is displayed.
2.	Click the Selection field from the dialog box.
3.	Right-click and select the Go to Profile Definition contextual command. The Profile Definition dialog box is displayed.

4.	You can define whether you need the Whole geometry, that is the whole sketch, or sub-elements only. For the purposes of our scenario, check Sub-elements if not already done.
5.	Select an edge.

	The sketch name as well as the edge name appear in the dialog box. The application also previews the pad.
6.	Click Add to add another element.
7.	Select an edge belonging to another profile. The application now previews this pad too.
8.	Repeat steps 4 and 5 using an edge belonging to the third profile.
9.	Select edge2 from the starting elements field and click Remove to remove the associated profile from the selection.
10.	Click OK to validate your selection. The Pad Definition dialog box reopens. You then just have to enter the parameters of your choice to extrude two profiles.
	Optionally click Preview before confirming the creation.

	If you encounter complex profiles causing ambiguity cases, the application lets you determine which lines you want to use as illustrated below:

	CATIA detects an ambiguity as shown by the red symbol : the user can determine three different lines from this point.	The user has defined the line he needs to end the selection.