I have a PCB layout as shown. My question is can I route the PCB between the copper pads? The purple colour is solder mask. From what I know solder mask is the green stuff on a PCB which covers the copper, determines where the copper is actually exposed. So once copper is removed on the board, it is coate with a solder mask which is then removed at certain places. Is it okay to route between these red copper balls?
Looks like you have a 0.5mm-pitch BGA. You may even have to use via-in-pad and 6 layers to get this to work. Below is a suggested 6-layer layout from Lattice that does not require via-in-pad.
With the solder mask as shown, you should not route between pads on the top layer. The reason is that if the solder mask relief for a pad also exposes a track connected to a different net, then there's a high risk of the solder ball bridging between the pad and the track and causing a short circuit.
For a 1-mm pitch BGA it's usually possible (with a high quality pcb shop) to reduce the solder mask reliefs enough to allow routing at least one 4 or 5 mil track between pads.
As the comments and other answers have said, if this is a 0.5-mm-pitch BGA, you'll very likely need to use higher-cost processes, such as multi-layer board, narrow tracks, via-in-pad, etc. to route into this device.
It all depends on your chosen design rules.
Your PCB manufacturer will have several sets of rules for the minimum width for your pads and tracks, and the minimum spacing between tracks and other features. They will have a cheap set of rules, with large dimensions, that are easy to achieve. They will also have a premium set of rules, with tighter dimensions that they will need to work harder to maintain (more careful alignment and control of etching conditions). The thickness of copper can also affect these distances, thicker copper means more undercutting. The last time I looked, 4 thou was expensive, 8 thou was easy. YMMV.
Decide how much you want to spend on their process, and get the correct figures for minimum track and gap widths. Then measure the distance between the pads and see whether the numbers add up. Or put these figures into your layout program DRC (Design Rule Checker), route a track between the pads, and see whether it's allowed.