When I need to “play around” with an assembly, I just create a copy of the assembly (not of all the individual parts) and do whatever I want to the copy. Simplistic, but it works.

WDG57 is right - since ProE creates 'parametric' file associations, it is not possible to have a drawing that is not directly associated with a component or assembly.  Drawing files do not contain part geometry...they only show what is in the .prt or .asm file.

WDG's method can work, if you don't mind duplicating the data.  However, the way I would set it up is to create a family table in the assembly.  Within the family table, you can vary an assembly constraint, dimension, etc which represents the change in position/size of the component(s).  This new instance can have its own drawing, independant of the original drawing.

Also, here is an easy way of creating an instance drawing when a drawing of another instance already exists:
Open the original drawing and select Save As... - for the new drawing name, enter the name of the instance you created.  Then open the new drawing and select Views>Dwg Models>Replace, and select the instance (if family table was set up, it will automatically pull up the list of available instances).  New drawing is now linked to the new instance, and all parametric linking is still maintained without creating redundant data.

I suggest that you have a firm grasp of Family Tables before doing this, because a slight lack of attention to detail can yield very confusing mistakes that are difficult to track down and resolve.

Recneps