(Not) Impossible to separate AGND from DGND

Question

I'm designing a USB-MIDI board and I decided to go for 4 layers. Since the digital and analog inputs (i.e. potentiometers and momentary push buttons) are distributed throughout the board, it's virtually impossible to separate AGND from VGND. What can I do to minimize noise?

I was thinking about routing the return paths of the digital inputs on one of the signal layers and use the ground plane for analog ground only but I don't know if this is a smart thing to do.

Edit: Thank you for your helpful answers and comments. What I took from that is: It is totally ok to have a single ground plane for analog and digital signals but you should arrange your components wisely and shape that plane in a smart way. Since the layout of the components is mainly determined by the layout of the hardware user interface I cannot do much about that. But of course I can shape that plane.

When I asked that question it was pretty early in the morning and I probably didn't provide enough detail. My PCB has a socket for a Teensy 3.6 which serves as MIDI USB controller and controls a few mosfets as power switches for other attached devices (2x 3 amps). The Teensy has an AGND and a DGND pin. Both grounds are connected inside the Teensy board. I just realized that I indeed could separate AGND from DGND but the shapes of those planes would look a little bit unusual:

It is my first PCB ever (yes I know that's a little bit ambitious for a first project) and I'm not sure if this is a smart approach. Thank you for your help!

Answer 1

For what it's worth, at my last two jobs I've had the pleasure of working with a super-talented electrical engineer (different person at each company), and in both cases the engineer's preferred design approach was to use one single ground plane for everything. Yes this runs counter to the conventional wisdom of how to lay out circuit boards, and they freely acknowledged that. But these were smart, methodical, informed, well-educated individuals who consistently produced great-quality designs, using just that one plane for everything both analog and digital.

Now unfortunately I don't have deep knowledge of how they worked their magic, but I can pass along the bits that I do know:

1. A good ground plane might be all you need.

The use of double-sided or multilayer PCBs with at least one continuous ground plane is undoubtedly one of the most successful design approaches for high-performance mixed-signal circuitry. Often the impedance of such a ground plane is sufficiently low to permit the use of a single ground plane for both analog and digital parts of the system.

Source

2. Understand all your return current paths. Your signal, plus the return current, forms a loop. The signals on your board will couple to one another through these loops -- if you keep these loops small and well-separated, then there will be very little coupling. Source Remember that the loop at low frequencies may look different than the loop at high frequencies, since at low frequencies the current will follow the path of least resistance, and at high frequencies the current will follow the path of least inductance. Source

3. Minimize the chance for your circuitry to introduce noise in the first place. This means having good decoupling located right at your ICs (and make sure high frequencies are sufficiently covered -- what's the self-resonant frequency of that capacitor?) and, possibly more importantly, put a little series resistance such as 10Ω right at the output of your drivers to soften the edge rates on your voltages (and also help to mitigate the current spikes on your power supply).

4. Be meticulous, detail-oriented, and fussy. Worry about the smallest details of getting the signals and routing just right. Follow the IC vendor's recommended layout rules exactly.

It's not easy -- if it was easy, everyone would be doing it -- but I've seen that it can work, and work quite nicely.

EDIT

My Google-fu did not work out for me earlier, so I had to make do with my second-hand perspective as stated. Now that I see this excellent answer from @peter-smith I can just say "yes. this."

Answer 2

Upvoted the correct answer of Mr. Snrub that is often better to have one single plane.

But would like to add that in case of separate ground, they should:

• Be connected underneath the ADC (or the device that does the bridge to the digital part).
• If you have several of those, I do a bridge underneath each of them, but keep them all in the same side of the plane and close together.
• Avoid plane overlapping at all cost.
• No trace shall go through the GND and AGND plane gap besides on top of the connection.
• Place the plane ground on the edge of the board and not the middle.
• Use filtering on the VDD with ferrite and caps

I had pretty good luck with those few rules measuring uV signals on 16bits at several hundred kHz with very low noise.