Broken-out Section
A broken-out section view cuts
away a portion of an assembly in a drawing view to expose the inside.
Cross hatching is automatically generated on the sectioned faces of all
components.
A broken-out section is part of an existing drawing view, not a separate
view. A closed profile, usually a spline, defines the broken-out section.
Material is removed to a specified depth to expose inner details. Specify
the depth by setting a number or by selecting geometry in a drawing view.
You cannot create a broken-out section on a detail, section, or alternate
position view. If you create a broken-out section of an exploded view,
you cannot collapse the exploded view.
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This example shows (1) wall thickness and shaft and (2) how the shaft
is welded to the cap: |
Broken-out section of a pictorial (isometric, trimetric, dimetric) view.
The depth is normal to the sheet: |
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To create a broken-out section:
-
Click Broken-out Section
on the Drawing toolbar, or click Insert,
Drawing View, Broken-out
Section.
The pointer changes to 
.
If you want a profile other
than a spline, create and select a closed profile before
clicking the Broken-out Section
tool.
Sketch
a profile.
Set options in the Section
View dialog box. If you do not want to exclude components or fasteners
from the broken-out section view, click OK.
Set options
in the Broken-out
Section PropertyManager.
Use 3D
drawing view mode to select an obscured edge for the depth of a broken-out
section view.
Click OK 
.
To delete or edit a broken-out section:
Right-click the broken-out section in the FeatureManager design
tree and select one of the following.
Delete.
Edit Definition.
Set options in the Broken-out
Section PropertyManager, then
click OK .
Edit
Sketch. Select the sketch entity and edit it, then close the sketch.