Creating a Section View / Cut with Profile Defined in 3D

In this task, you will learn how to create a section view or a section cut using a 3D profile as cutting plane.

Section views / section cuts are usually created using a cutting profile as the cutting plane; such a profile is typically driven using concentricity or parallelism constraints. Defining a profile in 3D to create a section view / section cut enables you to make the profile associative with the geometry, and therefore to drive this profile using dimensional constraints, for example.

Open the GenDrafting_part.CATPart and the GenDrafting_front_view.CATDrawing documents.
Tile your windows vertically to see both your part and the related drawing.

1. In the Part window, click the Sketcher icon

and select the xy plane as the reference plane. You are now in the Sketcher workbench.

2. Click the Profile icon

and sketch the profile you will use as cutting plane. For the purpose of this exercise, make sure you sketch your profile using orthogonal lines.

3. You can now create dimensional constraints between your profile and other elements. Click the Constraint icon

4 Now, click a vertical line and the edge of the part to create a dimensional constraint between them.

4. Exit the Sketcher workbench.

5. In the Drawing window, click the Update icon to update the view.

6. Click the Offset Section View icon

from the Views toolbar (Sections subtoolbar).

Depending on the type of profile you sketched and on the type of section (offset or aligned) you want, you can select another icon on the Sections subtoolbar. If the 3D profile is not valid for generating the appropriate view, you will not be able to select it. In this case, you will need to select another icon.

7. Select the profile on the 3D part.

The cutting profile is automatically displayed on the front view as well as a preview of the view to be generated. Positioning the section view amounts to defining the section view or the section cut direction.

8. Click to generate the view.

	You can modify the section view / section cut by editing the 3D profile. After doing so, don't forget to update the drawing.
	When editing a 3D profile, make sure that you modify it in accordance with the type of section (offset or aligned) you created: if an edited profile is invalid when you update a drawing, the associated section view / section cut will not be displayed (an error symbol will appear instead).
	If you delete the 3D profile and then update the drawing, the section view / section cut will not be deleted. The profile will no longer be associated with the geometry. You can subsequently edit the profile directly in the drawing by double-clicking it.
	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.