Balancing copper on inner layers of PCB
When a multilayer board is produced, the copper structures of inner layers and outer layers are manufactured in a different way. If an inner layer should be 35 µm thick, the take a thin board with 35 µm copper on both sides, add fotoresist, expose thru a film with the structure, develop the resist and etch all unwanted copper away. 

The outer layer are done different, because the drill wholes should be plated with copper. They use a copper foil with only 17 µm for the outer layers and add another 17 µm of copper by galvanic deposition. But all areas where you want no copper are covered with resist. The galvanic deposition of copper is done only at uncovered traces and copper planes and inside the drill holes. But you want all traces to get an equal deposit of copper. If there is a single trace in an area of the board only, all copper from the galvanic anodes goes there and this trace get much more copper than only 17 µm. At other areas of the board there may be a very dense population of traces. The copper from the anodes inside the galvanic bath spreads to all traces there and the deposition of copper will be less than 17 µm.

If the outer layers are structured with a good balance, you will get an equal deposition of copper to the whole area.

Balancing the copper is recommendable only for the outer layers of the multilayer if the inner layers are structured by pure etching.

But you should ask the board manufacturer about his recommendations for inner and outer layers.