As far as I understand, through holes in PCBs are often plated, hence the term PTH. Letting red denote copper, the first figure shows a through hole which is plated, and the second figure shows one that is not. The thick black line is the pin of a component, while the silver denotes solder applied. I can't figure out why the copper plating (otherwise known as the barrel) is needed - can someone explain why?
With through plating:
Without through plating (why isn't this the norm?):
In order for your scheme to connect the top and bottom layer, TWO conditions must BOTH be met:
In very many cases the top pad of a thru-hole component is NOT accessible because the body of the component covers it. So that is not practical.
In MOST cases there IS NO component lead at all where you need to via from one side to the other. Inserting short bits of wire and soldering BOTH SIDES is simply not practical even for manual assembly not to mention automated assembly as virtual all modern gear comes from.
It doubles the effort to require soldering to BOTH sides of even a thru=hole component lead. That takes double the assembly time, and greatly increases the chances of assembly error. It is simply not reasonable at any level.
Your first image is not completely accurate. The solder should also be sticking to the plating in the hole, and not just connecting to the top and bottom layers of metal. That is to say, plating offers improved mechanical stability and increased joint strength due to the much larger surface area available for soldering.
If you have plated-through holes, tracks on both sides of the board (and any internal layers) are connected without any further action.
Holes exclusively for this purpose are called "vias" and may be smaller than regular holes for component leads.
This makes manufacturing any board too complex to be single-sided, easier and usually much cheaper than otherwise possible, since no extra effort such as inserting jumper wires or soldering on both sides is required.
It also makes design and layout of double-sided boards much easier since you no longer have to strain to minimise the number of tracks on the "other" layer, or minimise the number of jumpers, or ensure crossings between layers aren't underneath components.
And that allows you to increase the board density and use smaller boards, cheaper enclosures, etc...
It also allows the PCB manufacturer to perform "bare board testing" of every one of these interconnections before any components are added - thus eliminating many defects. (Some PCB makers perform bare-board testing free of charge).
Plated holes give you all this before even considering how you actually solder a component to the PCB - though it offers advantages there too...
Most circuit boards are soldered by machines. Solder wave in the case of through-hole boards. The solder wave is a ripple in the surface of molten solder that the board is dragged through using a conveyor. It passes over all the pads and trimmed leads on the bottom of the board. It does not solder the top of the board. Soldering leads on the top would not only require them to be accessible but would require hand labor to solder each one. This would not be cost-effective in the case of production quantities- any tiny saving in the boards would be dwarfed by the hand labor required, not to mention the cost of a design constraint that requires all the leads to be accessible on the top (think of connectors, electrolytic capacitors, IC sockets etc.)- that means bigger boards, bigger housings, more packaging, more shipping costs, more shelf space etc.
So the standard for 2-layer boards is plated-through holes, and at some small additional cost you can have unplated holes as you mention. It's an additional operation so it costs more- the holes have to be drilled after the plating operation. Probably most boards have some unplated holes as well- they tend to be better for things like pressed in pins because the dimensions are more controlled.
There is nothing stopping you from ordering boards with unplated holes everywhere if you enjoy the extra soldering (though they may think you made a mistake and 'correct' it for you if there are connected pads on either side of a hole) but you won't save any money.
Most mpdern electronics has some measure of SMD (surface mounted) components, the leads of SMD parts lay flat and don't go through the board. Plated through holes are a handy way of linking top to bottom. That way, the top and bottom layers come connected from the factory so you dpn't have to connect them yourself. They also make a good low thermal resistance path when you want to use the board as a heatsink (plain old FR4 makes a terrible heatsink). Where PTHs are real useful is when you have more than two layers and you need to connect them or when you have parts with really small pads that need to be connected to another layer, pads far to small or too numerous to connect them manually (OSH park will happily make you a 4 layer PCB with 0.25mm holes with 0.45mm pads, and that's at hobbyist prices, cutting edge IT stuff can have 10-20 layers and holes less that 0.1mm wide that only go part way through a PCB). You don't have to use PTHs but the technology os at a stage where it adds only a few percent to the overall cost of a professionally made board.
I have made, for the sole purpose of saving money, two sided board without PTH (as the second figure of your question). The board was very simple, but testing was painful! - Testing net connectivity on the board was impossible without soldering first all the components - Bad soldering of the components (the mounting was by hand) meant electrical connectivity lost, so I have to re-check all the joints several times
After that experience with a two layer but no vias PCB, I opted for paying a little bit more but having faster testing times.
So, the point is: you can go without VIAS, but if you are talking about any real, practical project, you will be sorry of not having them.
Richard answered the question well, but WHY a plated-through hole only needs to be soldered from one side hasn't been properly explained in this thread. The surface tension of the solder wicks it along the barrel and component lead all the way through the hole, providing a connection that is both electrically and mechanically solid. If the hole isn't plated through, the circuit board material is resistive enough to solder that it won't wick through and reach the other side, so both sides need to have solder directly applied.
Structural instability issues can arise in the highly likely chance that air is trapped between the two solder layers on a non-plated-through board.
