an issue with part flexibility

A family table with an instance for each configuration would handle this within the part model.

https://support.ptc.com/help/creo/creo_pma/usascii/index.html#page/fundamentals/fundamentals/fund_ten_sub/About_Family_Tables_1.html 

Your use of the word flexibility in this context may be misleading to other users. Flexibility has a specific meaning for Creo Parametric functionality, and I do not think it applies to your situation based on your description. Flexible components are the area where the term is used.

Flexibility, in terms of intended functionality, is supposed to be an item like a spring or o-ring that is in one shape or form with in a free state but takes another shape or form when in an assembled state. It can only have that "alternate" shape when assembled.

I do understand (or I have done/seen/used/drawn) something very similar to what you are asking. A spring drawing showing a free state, a compressed state/ stretched state. Usually along with some values of what the expectations are for those states. I have in the past simply used sketched curves in the model to show those.

Similar to the other responses, I have made family tables (create separate instances) where the assembly "uses different" parts, which are the same part but modeled in a different state - extended or compressed. Then I just use the two instances of the same part as needed in the drawing to show the two "states" of the assembly.

If you're "adding and subtracting" features, that's a Family Table part and you're swapping out instances.  As mentioned below, there is actual "Flexibility" which, as mentioned above, can do things like give you compressed springs, o-rings, but also fill out your BOM differently.  For instance, my fasteners can be used where you can enter a mil-spec and mil part number, or you can use a vendor name (i.e. McMaster-Carr) and part number, and depending on what you enter it will fill out the BOM however you want, and you can change the material and finish however you want as well.  Or you can not use those parameters at all and you'll simply get the standard description (i.e. .250-20 UNC-2A X 1.500 LONG) in the BOM, useful for companies where you simply grab fasteners from a bin in the back and don't need mil-spec or vendor part numbers.

For what Dale mentioned you can create different "Simplified Reps" so that you don't get 2 different springs (if your assembly has different compressed heights) in the same BOM, but make sure the rep you want the BOM to represent is the current rep BEFORE you add the BOM table.  Repeat Region BOM tables take the parts in the current "Rep" to populate the table.  It's a little trickier than all that, but that's the gist of it.