Standard 3 View
The Standard 3 View option under
Insert, Drawing
View creates three related default orthographic (front, right,
left, top, bottom, and back) views of a part or assembly displayed at
the same time. For information on the orientation of the Standard 3 View,
see .
The view orientations used are
based on the orientations (Front,
Right, and Top)
in the part or assembly. The view orientations are fixed and cannot be
changed.
The alignment of the top and side views is fixed in relation to the
front view. The top view can be moved vertically, and the side view can
be moved horizontally.
The top and side views are linked to the front view. Right-click a top
or side view and select Jump to Parent
View.
For more information about arranging views on a sheet, see Moving
Views and Rotating
Views.
There are several ways to create a Standard 3 View drawing.
To create a Standard 3 View
when starting a new drawing document:
Open a
new drawing.
In the
Model View
PropertyManager:
Under
Part/Assembly to Insert, in Open documents, select a document, or
click Browse to locate a document.
Click
.
Under
Orientation, select Create
multiple views and click *Front, *Top,
and *Right. (You can also select
annotation
views.)
Click
.
Creating the Standard 3 View by the standard
method:
In a drawing, click Standard
3 View on the Drawing toolbar, or click Insert, Drawing View,
Standard 3 View.
The pointer changes to .
Select the model in one of these ways:
Select
a model from Open documents in
the Standard
3 View PropertyManager or browse to a model file and click OK
.
To add the views of a part, in a part window,
click a face, or anywhere in the graphics area, or click the part name
in the FeatureManager design tree.
To add the views of an assembly, in an assembly
window, click an empty region of the graphics area, or click the assembly
name in the FeatureManager design tree.
To add the views of an assembly component, in
an assembly window, click a face on the part, or click the name of either
an individual part or a sub-assembly in the FeatureManager design tree.
In a drawing window, click a view that contains
the desired part or assembly, either in the FeatureManager design tree
or in the graphics area.
Creating the Standard 3 View by the drag-and-drop
method:
The default view created when you drag and
drop a part or assembly into a drawing is the Standard
3 View.
Open a new drawing window.
-
Drag a part or assembly document from the File
Explorer, and drop it into the drawing window,
- or -
Drag the name from the top of the FeatureManager tree of an open
part or assembly document, and drop it into the drawing window.
The views are added to the drawing.
If you use this method to
insert a part or assembly that contains annotation
views, the Model View PropertyManager
opens, and a preview of one view appears in the graphics area. In the
PropertyManager, under Orientation,
select additional drawing views to insert, then click .
Creating the Standard 3 View from a hyperlink
in Internet Explorer:
In Internet Explorer (version 4.0 or later), navigate
to a location that contains hyperlinks to SolidWorks part files.
Drag the hyperlink from the Internet Explorer
window, and drop it in an open drawing window. The Save
As dialog box appears.
-
Navigate to the directory where you want to save the part, enter
a new name if desired, and click Save.
The part document is saved locally, and
the views of the part are added to the drawing.