How to calculate the size of ground plane we need to use in a PCB (printed circuit board) design
There are two aspects of a ground plane: its performance, and its appearance. The first is important. The second is not. Unfortunately, many people starting out concentrate on the second, to the detriment of the first.

A ground plane should be as big as it needs to be. That is, it should be present at or near* every connector, every IC, every supply decoupling capacitor, and every signal track.

A ground pour is not necessarily a ground plane. It can have the appearance of a ground plane. It's easy to do a pour as the last step laying out a board, it's difficult to check whether it does in fact connect all the points that should be connected. 

There are two ways to make a good ground plane. One is to lay out a ground track as you make the board, so that you can see it that it follows all the signals, visits every IC directly, before you confuse yourself with the pour. If you couldn't route the track, then the pour will not have made the necessary connection either! 'Letting the pour take care of that connection' is asking for trouble.

The other is to dedicate a ground plane layer, and then don't cut it up. Too often we via a track onto the ground plane layer 'just for a few mm' to ease tracking problems, and then another, and another. Done once or twice, with a short track, it's OK. Done excessively, it cuts the ground plane to shreds, and it can't do its job. You can via across breaks on the other side, but it's hard work to make sure you've caught them all, best not to cut in the first place.

There are only a few instances where a ground plane should not be, and in almost all cases, it's where a component's data sheet tells you not to. Near to a chip antenna, where the data sheet gives you a detailed footprint. Under the inverting input of a fast high impedance op-amp, where excess capacitance can hurt stability. Near to pins carrying dangerous voltage, opto-couplers will often tell you what distances are required for what voltages. 

*Near. For low frequency boards, 'near' can be quite big, without hurting performance. For RF boards and logic boards with fast edges, 'near' usually means directly underneath.