Im fairly new to laying out my own PCB's and have what may appear a stupid question...
But when should one switch from having GND routed just via tracks to using a plane ? I mean obviously, there is physical design reasons and often compentary reasons, but from a purely 'you should be using a plane' type scenario, when does one switch ? If it involves RF or sensors, should I just be using one anyway ??
Thanks for indulging me! 
I use a ground plane whenever it is practical to do so and a power plane too if I can. The advantages are many. A ground plane provides some shielding from external noise but probably more important it provides a much lower impedance at high frequencies which, together with the generous use of decoupling capacitors (100nf or so) really reduces the production of glitches and rf emissions.
Decoupling capacitors (between power and ground) are inexpensive. At least one should be located as close as possible to the power pin(s) of EACH chip.
Having a ground plane also means there is less copper to etch away. You use up less of your etchant.
and have what may appear a stupid question
It's not stupid it is in fact an area of fine judgement.
Generally with a four layer board you would always use a ground plane. However I suspect we are talking two layer here.
Ground planes are better but not if they are broken up too much. A broken ground plane will give you "ground bounce" problems as you can get multiple paths of current flow. In this case you are better off using a star topology and ground tracks.
This becomes more important the higher frequency you go or the more analogue you go (for A/D converters) and also the higher current you have flowing through the system.
It could be that you try one configuration and it proves to be unsatisfactory and you have to lay it out again.
Thanks Mike! Indeed I was referring to two-layer boards - I haven't gotten to needing the benefits of 4-layer boards, and figured I'd avoid the hassles (and costs) of potentially creating my own capcitance with 'unnecessary' power and ground planes... I'm still very much learning.
Could you possible point me in the direction of some good references, or perhaps expand a bit on the A/D side of things? My current project is relying entirely on the onboard ADC. I realise for better precision in a datalogger, I am better of shifting to using a higher resolution ADC (12-bit seems to be the best I can reasonably find tho.. surely there is higher available cheaper).
I have been researching a tiny bit about the differences of AGND and DGND, and plan to separate the two planes except for a small bridge. I was also, just because I thought it would be 'a good idea anyway' have mitred the corners of the GND plane anyway to try to reduce unnecessary reflections of current around it (not sure if this does anything - it seemed a good idea at the time I'm purely assuming but the 'current' would flow across the plane like water across a similar flat surface - the more bends or 'extrusions' you have to the polygon the more there will be reflections around, jitter etc in the harmonics..., so if you do bridge, you should channel down gently to a bridge (unless its intentional and you want to present a high resistance, such as AGND and DGND??).
Im probably getting well ahead of myself anyway at this stage - But my curiosity has gotten the better of me.
I appreciate yours and everyone elses responses so far!
potentially creating my own capcitance with 'unnecessary' power and ground planes
That is good coupling, in effect it is like distributed supply decoupling. What can be bad is to inject signal noise into the ground plane and so sometimes you want to back off the fill under large signal tracks. There is a technique called a guard track. Here a signal track has ground track on one or both sides, this has the effect of screening without injecting too much signal into the general ground plane.
Yes thinking of grounds in the way of flowing water is good.
If you are interested in the analogue side rather than the digital side then yes separate analogue and digital grounds are a good idea. Each having it's own decoupling. Keep large signals away from the analogue ground and put guard tracks round the analogue pins.
I don't know of a book as such although there are bound to be some and they will be very expensive. The best place to look is in manufacturers data sheets and application notes. These tend to have track layouts you can follow. Look at the data sheets for A/Ds instrumental amplifiers and switch mode power regulators all are layout critical components.
The other thing to watch is vias, when putting vias in ground planes then don't just use one but several. We say "stitched with vias" and some ground planes are pepped with them on a regular grid.
The other thing to watch out for is copper balance. This can be important if the boards are being mass produced. Basically don't have great areas of the board with planes and other large areas without especially on different boards as this can lead to warping of the boards as they go through the oven.
Have a look at these links:-
Cheers ! PCB Layout Guidelines and Tips is very helpful
By 'guard track around the analog pins' I assume you mean literally that.. a track connected to gnd that surronds the signal pin ?
a track connected to gnd that surronds the signal pin
Yes, either surrounds it on both sides or tracks along side it on one side.