Have you ever had an assembly that uses a component that you didn’t want to show in the BOM but you still wanted to see it in the drawing view as “see through”? The most common use for this that I can think of is showing a part that is being held in place by a fixture. You need to have the fixture components in the BOM, but you do not want to show the part. However, on the drawing views you want to show the part for orientation purposes.
By utilizing the Alternate Position function, you can show your part as “see through” and not have it included in the BOM.
To accomplish this, first create your assembly with the part in it (this is automatically the Default configuration). Then create a configuration called “Part Not Visible” (or something similar). Suppress the part in the Part Not Visible configuration.
In a drawing, create a drawing view using the Part Not Visible configuration.
Select the newly created view and then go to Insert=>Drawing View=>Alternate Position.
In the PropertyManager window, select “Existing configuration” and select the Default configuration.
Your drawing view now has the “Part” shown as phantom lines but “see through”
Now, when you create a BOM from this view, the “Part” will not be in the BOM (just make sure the BOM is referencing the Part Not Visible configuration).