Creating an Aligned Section View / Cut

This task will show you how to create an aligned section view and/or aligned section cut using a cutting profile as cutting plane.

An aligned section view / cut is a view created from a cutting profile defined from non parallel planes. In order to include in a section certain angled elements, the cutting plane may be bent so as to pass through those features. The plane and feature are then imagined to be revolved into the original plane.

Before You Begin, make sure you customized the following settings:

Grid:
De-activate the Grid icon from the Tools toolbar (bottom right).

View names and scaling factors:
Go to Tools->Options ->Mechanical Design -> Draftingoption (Layout tab) and check the View name and Scaling factor options.

3D colors inheritance
Go to Tools->Options->Mechanical Design->Drafting option (Generation tab) and un-check the 3D colors inheritance option.

	Open the GenDrafting_aligned_view02.CATDrawing document.
	1. Click the Drawing window, and click the Aligned Section Cut . If desired, you can also click the Aligned Section View icon from the Views toolbar (Sections subtoolbar).

	2 Select the points and circles required for sketching the cutting profile. If you are not satisfied with the profile you create, you can, at any time, use Undo or Redo icons. Note that SmartPick assists you when creating this profile. The section plane also appears on the 3D part and moves dynamically on the part. 3. Double-click to end the cutting profile creation.
	Positioning the section view amounts to defining the section cut direction. The cutting profile is hole associative.
	4. Click to generate the view.
	You may modify the hatching pattern by right-clicking the section view and selecting `Properties` from the contextual menu. You will then display a `Properties` dialog box in which you will either select a new hatching pattern or modify the graphical attributes of the existing hatching pattern. Please refer to Modifying a Pattern.