Can I lay traces on internal layers of 4 layer PCB?
Tip. Keep ground as an inviolate layer, and use the 3 other layers for signals and power. 

Treat power as a signal. While there are theoretical benefits to having a power plane, it is rarely worth it. The cost of dedicating a whole plane to power is too high, in terms of real estate. The time saving of 'not having to think' about power distribution is actually a problem, because it means that you tend not to think about power distribution!

A good layup is critical signals on the top (where you can keep an eye on them), ground as layer 2, then layers 3 and 4 as a strict Manhattan grid of power and less critical signals. 

The point about using a Manhattan wiring grid is that you always have a consistent way to get from A to B, you never have a tricky rip-up and reroute of half the board, late in the layout process. Those are the frustrating times when some people yield to the temptation to 'just run a little track through the ground plane', then you do it again and the next thing you know, the ground has fallen apart like a lace curtain.

Route power like this. Put a bulk electrolytic capacitor at the power entry to the board. Put a 10nF at every package power pin. Now think. Where can you tolerate voltage drops? Where must you have isolation between groups of components conducted via the power rails? What is the power consumption of each block. Now route tracks sufficiently wide for the current, and use series resistors, inductors, ferrite beads, or LDO regulators to achieve the desired rail voltages and inter-block isolation.

You don't always need a ground plane of course, only for RF and very high speed logic. A good alternative is to use a Manhattan pair of layers to lay an XY grid of ground tracks, connected at every intersection. Then you have 2 clear layers and two half layers for the rest of your signals and power. If you have a few critical signal tracks, then you can add a local ground under just those few.