Shield in Inner Copper Layer
Is this approach is right? Is it good idea to have SHIELD copper in
  the Inner layers?


I do a similar setup with on a PCB with shield ground, with the shield ground tied to a fastener. This allows for spurious currents such as RF or ESD to have a current return path through the shield and then the chassis and not through the board. Having a shield ground setup in this manner can be good for many designs.

However, I usually keep my shield ground on one side of the board, and don't have it overlapping any other planes. The thinking behind this is capacitance between layers could potentially be a way for noise to be introduced to the board. 

The main thing to worry about is the cross capacitance between layers. 

\$ C=\frac{\epsilon_r\epsilon_0A}{d}   \$

E_r for most boards is 4.5 to 4.8

For a standard for layer board the distance between inner planes is about 0.12mm and the inner most layers (or core) it is 0.5mm

This translates to 0.2nF between 1sq in of copper for the inner layers and 0.05nf between 1sq in of copper for the two inner most layers.



Source: https://www.pcbcart.com/pcb-capability/layer-stackup.html

So ask yourself, if I increase the capacitance between the planes will this be a problem for my design? 

I would think for ESD it could become problematic, but hard to say without building and measuring (or a really accurate model). It would really depend on the RLC circuit formed by the inter-plane capacitance and the inductance (and slight resistance) of the main current return pathway through the chassis.

There is also the problem of RF with cross plane capacitance.

The ideal situation (IMO) is having separation between chassis ground and ground, this takes the headache of thinking of what would happen with capacitance between planes. But if your design cannot tolerate this kind of design (which looking at it looks like it would be difficult to separate the planes) then go with something less ideal.