Ah, there's the problem -- you made two different symbols. Kicad won't let you annotate two symbols with the same reference designator.
What you need to do is to make a multi-unit symbol. In the schematic library editor, after you choose to make a new symbol or edit an existing symbol, click the icon that has ABC and an op-amp and gear. This opens the Properties dialog. Under the "Options" tag, look for "Number of Units." For a symbol with two parts (like a dual op-amp), set that to two. For your big part, set that to however many different symbols you want. Also, make sure that "All units are not interchangeable" is checked.
Now your menu bar on the top will have a drop-down list with "Unit A" showing. Pull down on this, and you'll see four units if you've defined your symbol to have that many.
Start drawing the symbol's outline. Note, though, that as you draw lines and such, you have to make sure that in the "Sharing" option for those things, the "Common to all units in component" option is not checked. (Double-click a line or arc to see its properties.) Otherwise, as you select the different units, those lines will appear for all. There is a similar option for pins (double-click on a pin, look for "Sharing").
You will quickly see an annoyance: the reference designator and the value fields will be in the same place for all units. This means that in some units, the refdes and value might be in a bad location. Don't worry about that, because when you place the individual units on the schematic you can move those two fields to a better location.
Another annoyance: you can't copy and paste between units.
When you're done editing, save the symbol to your favorite library. You should be able to place the different units on different sheets, give them all the same ref des, and the netlister should be happy.