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 First Angle and Third Angle Projection .

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:

1. Open a new drawing.

2. In the Model View PropertyManager:

   1. Under Part/Assembly to Insert, in Open documents, select a document, or click Browse to locate a document.

   2. Click .

   3. Under Orientation, select Create multiple views and click *Front, *Top, and *Right. (You can also select annotation views.)

   4. Click .

Creating the Standard 3 View by the standard method:

1. In a drawing, click Standard 3 View on the Drawing toolbar, or click Insert, Drawing View, Standard 3 View.
   
   The pointer changes to .

2. 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.

1. Open a new drawing window.

2. 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:

1. In Internet Explorer (version 4.0 or later), navigate to a location that contains hyperlinks to SolidWorks part files.

2. Drag the hyperlink from the Internet Explorer window, and drop it in an open drawing window. The Save As dialog box appears.

3. 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.