But Kai I was worried only about one thing...

I remember I have read it somewhere can't remember where exactly. It says when two tracks are running close to each other than the effective inductance of the traces is reduced to half.
Wont it hamper this phenomena if I increase the distance between traces in order to introduce ground in between them.

Dear Prahlad,

two different digital signals must always be separated by certain distance, so that toggling of one line will not propagate to other line due to charge injection via stray capacitance. If both digital lines are very close to each other and you toggle one of the lines very quickly, then you will notice a very fast spike on the other superimposed to its signal. If noise margin is violated, then you will become trouble...

One way to prevent such cross coupling is to shield the different signals to each other, by routing a solid ground plane between them, exactly as you did it with your latest changes of layout. It's imortant to use many vias there, to keep the impedance to solid ground plane of bottom layer very small, also exactly as you did it.

Another way to shield these signals, is to route them over a solid ground plane. But this is only helpful, when distance to solid ground plane is heavily decreased, like it is used with multilayer boards. It can be calculated, that the stray capacitance between the signals decreases to the same amount as the capacitance between signal and ground plane increases! Multilayer boards provide a very effective shielding between digital signals by this methode.

Sometimes it can be seen, that bus signals are routed very close to each other, even when no ground plane is very close underneath. As long as the signals belong to the same bus, where all signals are simultaneously clocked, means toggled, then a bit stray capacitance can be allowed if source impedance of drivers is very low and bus timing is not too fast. Then, injected charge due to cross coupling can be removed again before data on bus is latched.

What you stated about signals, which should be routed very close to each other, is only valid for a signal and ITS ground return current! Assume you want to drive a load by applying a voltage signal to it. Then there will flow a current to the load and a current of same amount back. Both currents produce a magnetic field. If you keep the signal current and return current close together, then a big portion of resulting magnetic field cancels, because magnetic field of current to the load and ground return current have opposite signs!
If you route a digital signal over a solid ground plane, then the ground return current will always flow directly underneath the signal current, not elsewhere on the board. This is especially valid for the high frequency content of signal. It can be shown, that by this current flowing scheme resulting magnetic field is minimal. And as inductivity is defined as produced magnetic flux per current, this also results in a heavily minimized inductivity of according signal traces.

Advantage of using solid ground plane is, that for every signal current a ground return current path directly underneath signal trace can be provided and by this keeping all traces' inductivities small!

Kai