Question about power line on PCB
I recently made a small PC board design that can help to show how you can do a 2 layer board but still achieve a good GND plane. In the picture below the left shows the top side of the circuit board while the right shows the bottom side of the board. Notice how the bottom side has been filled in to provide a GND plane. 

 

Any connections to the GND plane simply drop down as a via or component through hole. Component leads that connect to the GND use a special thermal spoke type pad connection so that it is easier to solder these pins without the plane sinking all the heat away from the solder point. When doing your layout for the GND plane side it is important to minimize how much area gets cut up by routing on this side. Sometimes you can improve the cut up areas by adding connections on the top side that bridge the GND in places where it was cut too much. You can see a bridging strap of this type just to the left of the P4 reference designator on the top side. On the GND side you'll see two GND connected vias.

The top side of this design has examples of bussed power and filled plane power distribution. The filled part is a 3.3V plane comes from P1-1 and feeds to pin 1 on U1, U2 and U3 and some capacitors. There is bussed 5V power that comes from P3-1 and goes to C1, C2, VR1 and down to U4 through a larger sized trace on the back side. The output of the VR1 regulator is 2.5V that is bussed to C3 and C4 and then to pin 16 on U1, U2 and U3 and some additional capacitors. 

Notice how capacitors are placed close to VR1 and the U1, U2 and U3 ICs. Also the C9 bypass capacitor is placed right across the 5V/GND connections of the 434 MHz radio receiver at U4.

I used the free schematic/PCB CAD package called Design Spark for this design.