All I am doing is putting a screen around an existing 2 layer PCB.
But what about board-thickness, prepreg, epsilon-r, return path and core? Have a look into this
document or this
document.
(There are more documents from EMC labs out there, a lot of research about this topic.)
Don't think about GND-layers, think more about reference planes. Not only GND-planes offer a return path. You want to keep your signal close to their reference plane with a constant impedance. Also proper decoupling is needed.
Something to think about: The idea about GND-layer on the outer layers of a PCB is nothing new. But in all these years, with all these smart guys out there, no one is doing this (*). Also in HS-design classes something like this is not taught.
A PCB with SMT and GND-layer on the outside needs way more vias. This is not the best practice regarding density and signal integrity. If a signal changes reference plane it needs a path for it's return current nearby. With two GND-planes you can us a via connecting these two planes. With a GND-plane and a VCC-plane you need a capacitor and two via nearby. All not good regarding signal integrity and more board space.
Anyway, theoretically two GND-planes on the outside could reduce EMC. But in reality it is not worth the effort because components on this GND-layer consume all space. If your layout and design is so bad regarding EMC-emission that you need the GND-layers on the outside, you made something wrong.
What do books like "HS Design Black Magic" from Johnson and "Signal and Power Integrity" from Bogatin say about this? I'm not sure, but I don't remember they recommend this.
Simon, give it a try. Why not? Nothing bad about trying new stuff. But be aware it is not best practice. And always ask yourself "What would Johnson or Bogatin do?" or "What was taught in this design-class?" or "Am I really smarter than all these guys out there?"
No pun intended!
*) Anyone?
Edit: "OpAmps for everyone" chapter 17.2.3
There has been a lot of confusion in the past over what is the optimum order for PCB layers. Take, for example, a 4-layer board consisting of two signal layers, a power plane, and a ground plane. Is it better to route the signal traces between the layers, thus providing shielding for the signal traces – or is it better to make the ground and power planes the two inner planes?
In considering this question, it is important to remember that no matter what is decided, there will still be signals exposed on one or both of the top and bottom planes. The leads of the op amp PCB package, and the traces on the board leading to nearby passive components and feed-throughs will be exposed. Therefore, any shielding effects are compromised. It is far better to take advantage of the distributed capacitance between the power and ground plane by making them internal.
http://electronics.teipir.gr/menu_el/personalpages/papageorgas/download/2/YLIKO_MELETHS_2012/sloa089.pdf