0
\$\begingroup\$

Due to layout restrictions I may have to have digital signal at one side of the board, and analog signal at the other side. I used to separate them dedicating parts of the board for each, but not this time.

  • Board thickness: 1.6 mm
  • Layers: 2
  • Digital signal: 3.3/2.5/1.2 V LVTTL, up to ~30 MHz
  • Analog signal: audio ±1.5 V (output of op-amps in voltage follower mode powered from ±12 V), mostly human ear hearing band

I am worried if quality or integrity of one signal will be negatively affected by the signal on another side of the board.

Are my apprehensions having a reason to exist, or I am over-complicating things? Should I make 4-layer board with ground layer as "padding" between digital and analog?

In general, what should I be aware of if I will decide to continue with such design?

@MichaelKaras: Not possible to separate at this time, that's why I ask this question. I have to place audio jack in the middle of digital logic because putting it in other places of PCB will simply make it not accessible outside of chassis. Audio signal will be fed to the jack through airwires, thus in general there will be just several pads of analog signal, but there're digital wires at another board's side which I afraid may suffer.

\$\endgroup\$
6
  • \$\begingroup\$ How sensitive are the analogue signals? (e.g. high-z, n-bit ADC, etc.). Also, what frequency are both analogue and digital roughly? \$\endgroup\$ – Tom Carpenter Jun 17 '17 at 23:16
  • \$\begingroup\$ Rather than putting analog components on the bottom side and the digital signals on the top side you should strive to split the board left and right and place the analog at one end and digital on the other end. \$\endgroup\$ – Michael Karas Jun 17 '17 at 23:43
  • \$\begingroup\$ Not possible at this time, that's why I ask this question. I have to place audio jack in the middle of digital logic because putting it in other places of PCB will simply make it not accessible outside of chassis. Audio signal will be fed to the jack through airwires. \$\endgroup\$ – Anonymous Jun 17 '17 at 23:48
  • \$\begingroup\$ Is this a headphone jack or an audio line out or both? Line level audio isn't as sensitive as headphone level audio. \$\endgroup\$ – mkeith Jun 18 '17 at 3:07
  • 1
    \$\begingroup\$ You can probably do it with 2 layers. Just give some thought to where the digital return currents will flow and try to keep digital signals away from the audio. The most critical part is the op-amp input. The op-amp input is very high impedance, and any noise that couples into the op-amp input can ruin everything. Hard to say much more than that without really getting into the design. 4 layers will make everything better, but will increase the PCB cost a lot (on a percentage basis). \$\endgroup\$ – mkeith Jun 18 '17 at 15:27
1
\$\begingroup\$

First of all you must understand that the digital signals will have return signals directly underneath them on the opposite side of the board. You need to make sure that your analog signal traces are not running parallel to the digital return traces or you will have cross talk.

Also, you need to make sure that all signals have a solid reference plane on the opposite side of the board or you will have impedance mismatches and excessive inductance and radiated noise since the return currents will be taking paths around any cuts in the planes above/below them.

Ideally you should flood the top and bottom of PCB with copper that is connected to ground, just be sure to keep clearance from unmasked copper to avoid shorts. You can also drop vias connected to ground along the path of your analog signals to shield them as best as possible.

\$\endgroup\$
0
\$\begingroup\$

Are my apprehensions having a reason to exist, or I am over-complicating things?

Adding a dedicated ground plane can make a difference by:

  • Lowering the inductance of the return current pathway
  • Providing a shorter and lower resistance return current pathway
  • Preventing common mode noise that comes from daisy-chaining loads.

Problems that might arise from added inductance or resistance can be overcome on a two layer board with careful planning, but it depends on a variety of factors like board size, components, desired SNR. Another problem that can arise from a 2-layer board is antennas, which will make the design prone to failure if you need to pass FCC regulations. Some designs require a 4-layer board, because high speed digital or analog signals need a solid ground layer for transmission lines.

Should I make 4-layer board with ground layer as "padding" between digital and analog?

There are different ways to stack up a PCB, you can even have two grounds on the outside layers to provide shielding to the inside layers (which presents its own problems when routing signals).

Adding a ground layer between digital signal layers and analog signal layers does provide shielding between the two. If you see digital switching noise in your analog signals, then you may have some noise coupling and may benefit from a 4-layer design. If a 2-layer design doesn't have any problems, then don't change it.

When you add a ground layer adjacent to a trace, you are increasing the mutual capacitance from that trace to ground. If you think your design would benefit from this and its worth the cost then consider a 4-layer design.

In general, what should I be aware of if I will decide to continue with such design?

This question is too broad, books are written on this subject. Without knowing much about your design (like the layout or function) I can't comment on this. Get an EMC or PCB design book, everyone application is different, everyone signal and noise bandwidths are different. Come up with some requirements for signal to noise and make sure the design achieves that.

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.