Designing a Part in an Assembly Context

	This task consists of designing the part you have just added to the assembly. It shows how to access the tools required for designing components in an assembly context.
	1.	Double-click `CRIC_JOIN` in the specification tree to access the Part Design workbench.
	2.	Select the blue face as shown and click the `Sketch` icon to access the Sketcher workbench.
	3.	Now that you are in the Sketcher, click the `Normal View` icon in the View toolbar and sketch a circle on the face using the `Circle` command . Do not bother about positioning the circle.
	4.	Now to obtain the same radius value as the one used for CRIC_JOIN circular edge. To make sure that this circular edge and the circle share the same axis, use the `Constraints Defined in Dialog Box` command to create a coincidence constraint (select the circle -if not already done- and the circular edge, then click the `Constraint Defined in Dialog Box`command and check "Coincidence").

		After validating the operation, the circle is coincident with the circular edge. You must obtain this:
	5.	Exit the Sketcher and use the `Pad` command with the "Up to Plane" option to extrude the sketched circle. Select the blue face as shown to specify the limit of the pad.

		After validating the operation, you should obtain this cylinder: The part is designed.

		For information about Part Design and designing in context, refer to `Part Design` User's Guide and Designing in Assembly Context respectively.