Creating an Offset Section View / Cut

This task will show you how to create an offset section view/cut using a cutting profile as cutting plane. In sectioning through irregular objects, it is often desirable to show several features that do not lie in a straight line by offsetting or bending the cutting 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_section_view02.CATDrawing and GenDrafting_section_view.CATDrawing documents.

Before You Begin:

Make sure the front view is active (use double-clicking).

Delete the text assigned to the front view (right-click on the text and select Delete option from the contextual menu)

	1.	Click the Drawing window, and click the Offset Section View icon or the Offset Section Cut icon from the Views toolbar (Sections subtoolbar).
	2.	Select the holes and points 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 appears on the 3D part and moves dynamically on the part.
	3.	Double-click to end the cutting profile creation. OFFSET SECTION VIEW Positioning the section view using the cursor amounts to defining the section view direction. The cutting profile is hole associative.

	4.	Click to define the section view direction and to position the view on the sheet. The view name and scale appear on the generated view as you checked the `View name` and `Scaling factor` options in the `Options` dialog box. Even when the view is generated, you can edit and modify the section profile. For this double-click this profile and either invert or replace it.

OFFSET SECTION CUT: in this particular case, select a circular axis and double-click when you are satisfied with the position of the rotating profile that automatically appears on the 3D view.

creatingoffsetsectioncut204.gif (5609 bytes)

Positioning the section view using the cursor amounts to defining the section view direction. The cutting profile is hole associative.

creatingoffsetsectioncut204.gif (5609 bytes)

Click to define the section cut direction and to position the view on the sheet.

The view name and scale appear on the generated view as you checked the View name and Scaling factor options in the Options dialog box.

Frame
The frame of the active view adapts to the length of the cutting profile.

Hatching pattern
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.

Apply uncut specification
In an assembly, you can define that given parts will or will not be sectioned when generated into section views or breakout views.
In the Assembly Design workbench, select one part, then the Edit -> Properties command from the menu bar from and either activate or de-activate the Not cut in section views options.

In the Drafting workbench, modify the view properties (Edit-> Properties or Tools->Options) to define that the resulting views will or will not be sectioned.

You can insert Bill of Material information into the active view.

You can assign a line type to the view to be generated. For this, go to Tools -> Options -> Drafting (Generation tab), click the linetype switch button and select the desired option from the Linetype for some views dialog box.