Explanation of the moating technique in PCB design

Hi everyone..
I am new into PCb designing ..I came across a board while trying to study different methods of designing.
I have attached an image of gnd plane for a project (digital board) with multiple voltage references.I find single gnd plane is differentiated into different sections connected though a bridges in the plane.Why is it done like this.My guess is the components are grouped with respect to their voltage reference and signal flow and placed .Hence instead of creating different planes for gnd/split planes they have used this method.Am i correct?
thanks
[/img]

Re: Split Plane

What you are seeing is called a "moat" - like the moat around a castle with a drawbridge.

The purpose is to force return current through a specific path, and prevent it from flowing where it might interact with the return current from a more sensitive circuit. This sort of thing is frequently used in A-D and D-A circuits to keep the digital and analog returns separated.

You need to know what you are doing when you use this technique. By controlling the return path in this way, you are most often increasing the signal loop size. That signal loop can be a souce of EMI - both from inductive coupling, and from radiated energy.

It's a good tool, but should be used with full knowledge of the entire signal path.

Re: Split Plane

As House Cat remarked, this technique should be used with care. De-coupling the moated areas in this way may prevent noisy signals from combining at the board itself, but differences in the return currents, and return path impedances, will generate differential noise. (If the planes were connected together, then the noise would be common mode.)

Split Plane

Thanks for your replies...
So My guess is each moated area will be for components with different power signal , say +5v,3v etc.Then if i have to connect traces from from one area to another would i be creating a large loop if i took the trace across the slots or should i take the traces through the bridged area?
Is there a better solution to it than moated areas.Usually which one has better EMI perfomance?

Re: Split Plane

Yes, you are correct. Critical signals would be routed on the adjacent signal layer such that they passed over the "bridge". DC or low edge-rate signals can safely go over a split, but not fast risetime signals.

To pass over a moat, or a split, with the least amount of signal integrity impact, one would supply return path vias connecting either direct traces or other contiuous planes. The return signal would be forced to another layer, but the loop size would be minimized.

The ideal solution, of course, would be to use continuous reference planes for all signals. This is not practical in the real world. Even solid planes that we call "continuous" are punched through like Swiss Cheese with pads, vias, cutouts, etc. The use of multiple planes also inceased the board thickness, weight, and cost. You have to compromise, and one of those compromises is to use split planes.

Split Plane

Thank you
How do we decide the area to be poured,the minimum separation between the splits
...one more doubt...say for a mixed board (analog and digital) i have 2 dedicated planes for each analog and digital .What exactly happens if a Digital/analog trace pass through analog/digital plane.I have understood it is also done to decouple noise from each section .
1)Does EMI issues happen also because of larger signal loop
2)Is there a characteristic impedance issue
3) Is there a voltage reference issue which corrupts the signal?