Why use ground fill on PCB?

The occasions where it might not be wanted could be where you need electrical clearances for (say) mains connections, and there are some circuits that may not like a ground plane too close or may want it with certain control over it, e.g. where the slight increase in capacitance between other signals and ground could cause an issue, and RF transmission lines. Some circuits fall into the category where no ground plane is needed, but there is no harm to add it.

If you decide to have a ground plane, then if it's just on one side of a 2-layer board, then the board comes from the PCB factory slightly warped which can be annoying or might not matter.

If it were me, then generally my approach when adding a ground plane for surface-mount component boards, is to put the ground plane on the underside, and have most traces on top (component) side (and maybe some short traces on underside if needed), and then fill the top component side empty areas with ground plane but with some clearance from components, no need for it to get super-close to components or traces, and then a few via holes for stitching top and bottom. The top layer copper pour then is mainly to help with preventing the warping.

If I was doing a through-hole-only board and it had a ground plane, then I'd put the ground plane on the component side so that it's easy to access the other traces on the solder side. 

If the warping doesn't matter then generally there is no need to have a plane on both sides for 2-layer boards, a single side of ground plane would then be OK. The top plane could be a different voltage if desired, e.g. use it as a 5V power plane, it's up to you.

Aside from electrical reasons for ground planes, they can influence your PCB process in producing better quality cards, especially if you etch them yourself. When you have to etch a large area of copper to create a bare patch on a PCB it will etch slower than thin traces, so by the time the large area is clear of copper, the thin traces are over-etched. This is a reason to avoid large bare areas of PCB. Sometimes polygon fills are created using a hatched pattern to avoid large bare areas. If you fill everywhere with copper then you can save on etchant - it will take less acid to etch and it will get etched quicker - so all around cheaper, quicker and more eco-friendly.

It sounds all good right, but there are of course numerous problems with fills that warrant a larger discussion, which is why I don't use them unless they are electrically necessary.

Such as the extra design time needed, the fact that most CAD systems, even expensive CAD software, can't generate a perfect pour and can't flag all pour issues and often it is very difficult to edit a layout after a pour is done.

I can appreciate the ground fill on do-it-yourself PCBs. I haven't dabbled in that in 30 years but I do recall the scenario of over etching the traces and having to do repairs.

I was wondering about about the PCB manufactures. They are laying down more copper on a ground fill board so I would assume the cost is more.

I don't know the process for modern PCB manufacturing, I assume they start with copper clad FR4, mask it and "grow" the copper layer wherever it is needed, including vias, then grow solder to be used as a mask for etching away copper that is not needed. PCBs with more than 2 layers are more complicated, I don't know if the middle layers have copper growing stages. The shops I use don't seem to charge differently depending on the amount of copper surface added or removed. They seem to only care about the total surface area of the PCB and the number of layers. Maybe it is different for high volume orders.

You have it backwards, my friend. The copper is already on the board and gets removed by the process (except for plated thru holes). Therefore, there's no extra charge for ground planes and in fact, it costs the PCB mfgs less to make a board with a ground plane. as far as your question, I'm not sure I fully understand what you're asking, You can choose to make a layer ground plane or with not and if you choose ground plane, then you do nothing in the layout software. I use Altium Designer and it works that way. The other way is to not choose ground plane for a layer and then to add a fill. You can fill the entire layer and then it will be no different than if you have chosen that layer to be a ground plane, or you can make a simple shape like a rectangle or you can make a very complex shape. 

In my most recent layout on a 6-layer bd, I used a couple of layers for large ground fills, but I had several of them, each assigned to a different net. For example, I had a 3.3V, 1.2V, 5.0V, 12V and although they're not technically a "ground", they got fills to lower the impedance. This gave me the best of both worlds, heavy planes and multiple nets instead of just assigning those layers to "GND".

This is the process I am familiar with. It includes a copper plating step as well as copper etching step.

https://www.4pcb.com/media/presentation-how-to-build-pcb.pdf

I too started with this thinking. From the little I've learnt, I too discovered that it does not cost anything more to add a ground plane and that using a ground plane "shields" data lines from interference, especially if you plan to use high frequency switching signals, for example. Probably also of value if you plan to use analog. I believe if you have traces on the top layer, for example, then the trick is to try and place a ground layer immediately below it. Vice versa if traces are on the bottom layer.