This article describes how to create an Alternate Position View in a SOLIDWORKS drawing

To create an alternate position view:

1. Insert a model view of the assembly using the orientation needed for the Alternate Position View. Position the assembly in its starting position. 

2. Click Insert > Drawing View > Alternate Position.

• The Alternate Position PropertyManager appears. You are prompted to select a drawing view in which to insert the alternate position.

3. Under Configuration, choose either:
1. New configuration: A default name appears in the box. You can accept the default name or type a name of your choice.
2. Existing configuration: Choose from existing assembly configurations that appear in the list.
4. Click OK. The results are either:
1. New configuration - If the assembly document is not already open, it opens automatically. The assembly's view orientation changes to that of the drawing view. The assembly appears with the Move Component PropertyManager open and Free Drag activated. Continue to Step 5.
2. Existing configuration - The alternate position of the selected configuration appears in the drawing view, and the PropertyManager closes. The view is complete. No further steps are required.
5. Use any of the Move Component tools to move the assembly components to the desired position. In the PropertyManager, under Options, use Collision Detection and Stop at collision to stop motion. 

6. Click OK to close the Move Component PropertyManager and return to the drawing.

• The alternate position of the assembly configuration appears in the drawing view in phantom lines, and the Alternate Position PropertyManager closes. 

7. Create as many Alternate Position Views as needed using the same steps.