I know I'm a bit late here, and by now you've probably taken the advice to create another family table at the part level to modify the cross section parameters, and then use the family table at the assembly level to replace component by family member. This is a fine way of doing it, but FYI, it also would have worked the way you initially envisioned if you'd known the trick about flexible models and associated parameters.
You'd start by setting up pre-defined flexibility in the part file, for the cross section parameters you want to vary. (This is actually an optional step, you can make any part flexible at the assembly level, but it's good practice to advertise which parameters ought to be adjusted there at the part level.) This is under File / Prepare / Model Properties / Flexible. (In Creo 2, which I'm still using.)
After doing this, when you place this part in an assembly, you're prompted if you want to use the pre-defined flexibility. If you'd already placed the part, you would right click on it in the model tree and select "make flexible".
A dialog pops up next, where you specify new values for the flexible parameters to use for this instance of the part in the assembly. There is a hidden trick here you need to know about! On the bottom, click the "set displayed columns" button, and add the "Assoc. Param" column. No idea why that column isn't shown by default, or why you don't get associated parameters by default to begin with... Here, you assign parameters which are visible at the assembly level, that can be used to adjust these flexible dimensions or parameters at the part level. You can even use the exact same parameter names if you want; there won't be a conflict.
This is how you get multiple copies of the same part to look different when used in different places in the same assembly, without actually updating the original part at all.
Now, in the assembly level family table, you'll add item of type parameter, and "look in" component to find them.
The good thing about this approach is you don't have to deal with all the family table instances at the part level. The bad thing about this approach is that since you don't have those family table instances saved at the part level, whenever you open the assembly the first thing that has to happen is a regeneration of the parts to get the right shape, which can increase the time needed to open a large assembly. And if you have a specific combination of options that suppresses regeneration (for instance, with read-only components from Windchill), then they won't look right.
