Now you add the pin. The pin references the inner diameter of the barrel and the overall length of the hinge pieces. Once you reference an entity of one part (the barrel) to create an entity in another part (the pin), you create a reference in the context of the assembly. If you modify the referenced entity, the new entity updates to reflect that change.
-
Click New
Part
on the Assembly
toolbar.
-
Select the narrow model face on the front of the assembly. The new part is positioned on this face, with its location fully defined by an InPlace mate. An InPlace mate is a coincident mate that is added when you create a component in the context of an assembly.
A sketch opens automatically on the selected face.
Notice that Edit
Component
on the Assembly
toolbar is selected because you are editing a component in the context
of the assembly.
-
Select the inner circular edge of the barrel, then offset it to the inside by 0.25 mm.
-
Exit the sketch.
Click Rebuild
on the Standard
toolbar.
The components that you are not editing become
transparent.
-
In the FeatureManager design tree, right-click the new part, select Rename Part, type Pin, and press Enter.
-
Right-click Pin and select Save Part (in External File).
-
In the dialog box:
- Select Pin under File Name.
- Click Same as Assembly to set the Path to match the assembly path.
- Click OK.