How to separate analog and digital grounds is a contentious issue in electrical engineering. They don't teach it in school. Here is my take on the issue.
Keep analog and digital circuitry separate.
In board designs with high-speed data converters, it is important to keep digital noise out of analog nets. This means keeping lines with high digital edge rates as far as possible from analog lines. Return currents of digital signals travel back to the source IC on the nearest ground or power plane, following the path of least inductance. Therefore separating the planes under digital and analog signals can prevent digital return currents from inducing noise in analog lines.
High-speed data converters have separate analog and digital power/ground pins. A user new to high-speed data converters will often imagine the data converter has a boundary inside it separating the analog to digital portions. This makes intuitive sense because the designer rightly has an imaginary line on her board separating the analog from digital portions of the PCB. It seems like the analog and digital power/ground pins should be connected to their respective planes on the board.
Tie analog and digital planes together at the data converter.
Contrary to intuition, the analog and digital planes should be tied together as close as possible to the data converter, usually directly under the data converter IC. Noise present on the digital ground at the part cannot be isolated from the analog portion of the circuit by a high impedance connection between the two grounds. Doing so develops transient voltages across the two grounds and encourages return currents to flow through the data converter’s ground pins, which is clearly undesirable.
In the example above, blue represents digital ground, and red represents analog ground. There is a moat separating the grounds except for a tie under the ADC and part of the DAC. ADC and DAC manufacturers recommend tying the grounds together at a single point near their part.
Why do IC manufacturers put separate analog and digital pins on their parts if you can’t use them separately?
The IC die contains separate areas for its digital and analog circuitry, just as a PCB layout does. They are connected to the IC's pins using bondwires, which have some unavoidable impedance. This bondwire impedance plus the impedance separating the analog and digital grounds on the die make the analog and digital ground pins different from the IC designer’s standpoint. From the PCB designer’s standpoint, however, they should be tied together outside the chip with the lowest impedance connection possible. DC and AC currents can travel through the part from one ground to the other.
What happens if the analog and digital pins are not tied together?
The analog and digital pins are not isolated inside data converter chips, so current can flow from one ground to the other through the chip. DC currents and AC transients flowing through the data converter from one pin to the other can cause the data converter to behave unpredictably and is always undesirable. Usually it increases the chance for noise. In one extreme case I have seen, in which the ADC had separate power supplies for analog and digital power, the ADC did not work at all at certain temperatures.
There is a saying that if you're presented with a board with EMC issues and the schematic has multiple ground symbols, that's usually a good place to start looking for the source of the problems.
Data converter grounding is complicated.
If the design requires low noise, it’s a good idea to run it by the IC vendor’s field applications engineer (FAE). If the relevant portions of the design are highlighted in the CAD package, a FAE can provide quick feedback based on a screen capture. Even if the estimated annual usage of the IC is low, some IC vendors still provide great support. However, be prepared for the possibility that the FAE is most familiar with an eval board containing only the data converter in question and without the complications of a real-world design.
If there are still questions about the best way to tie planes together, different options can be tested by ordering a panel of boards in which each PCB has a different grounding setup. This requires some communication between the board designer, fab house, and contract manufacturer. The experimental knowledge you gain from testing multiple layouts in a single spin makes it worth the effort.Here