Detail View
You create a detail view in a drawing to show
a portion of a view, usually at an enlarged scale. This detail may be
of an orthographic view, a non-planar (isometric) view, a section view,
a crop view, an exploded assembly view, or another detail view.
The enlarged portion is enclosed
using a sketch, usually a circle or other closed contour.
You can set the default detail view
scaling factor. It determines the scale of the detail view as a factor
of the parent view.
Detail views expand in the FeatureManager design tree so that all components
and features are available.
To create a detail view:
Click Detail
View 
on the Drawing toolbar, or click Insert,
Drawing View, Detail.
The Detail View
PropertyManager appears and the Circle
tool is active.
-
Sketch a circle.
To create a profile other than a circle,
sketch the profile before clicking the Detail
View tool. Using a sketch entity tool, create a closed profile
around the area to be detailed. You can add dimensions or relations to
the sketch entities to position the profile precisely relative to the
model.
If you plan to create a Broken View,
you are advised to relate the sketch to the model.
As you move the pointer, a preview of the view is displayed if you
selected Show
contents while dragging drawing view.
When the view is where you want it to be, click
to place the view. You can edit
the view labels, and you can modify
the view as necessary. To remove any sketches that are imported to
the drawing, delete them in the FeatureManager design tree.
You can move a detail view to a different sheet than the
parent view.