Need help with a mixed-signal board layout and grounding

[hummusdude]

This is an audio pre-amp with a 2 band EQ circuit I found online. There are several digital controls for the gain that are surely overkill but I'm just having fun with different things. The main control is a dpot that controls the gain of the TL072 op amp. The board is 2-sided and the whole bottom is a ground plane.

It's powered by two sources... +- 25 VDC from the main power supply that feeds a couple of linear voltage regulators that supply the 2 TL072 op amps (pre-amp and summing amp), and a 5 VDC source to power the digital components. The design originally used a 5 VDC linear voltage regulator fed by the analog voltage supply but in bread boarding it I noticed it was running quite hot. So I opted instead to use a tiny wall wart SMPS to power the digital components.

This is my first board and I'd appreciate some input about a few things. I'm sure it could be done with a more elegant layout but I'm mostly interested in addressing noise and any other glaring problems that it might have. So my questions are:


1) Is there enough distance between the analog side on the left and the digital side on the right? Aside from the 4 analog signal lines that go to and from the dpot, the closest gap is around 6 mm. Because it uses a dpot I don't see any way to completely isolate all of the analog signal lines. I've read numerous sources about grounding and I'm a little confused on how to prioritize the placing of analog/digital lines.

One source says separate them by at least 20x the thickness of the board, which according to KiCad is 1.6 mm. If that's correct than that would mean it needs 3.2 cm spacing. I can make the board bigger if that is the best option. But that seems a bit out there. And what does that mean about dealing with analog signal lines that have to connect to the dpot?

Another says that the current return path of high frequency lines (>1 MHz) will tend to follow the digital signal lines whereas low frequency signal return paths tend to spread out and also go more directly to the ground connection point. I put the 5 VDC ground point for the digital components far away from the analog ground. The Arduino runs at 16 MHz so that seemed prudent.

The circuit was pretty quiet on the bread board except for some 60 Hz hum which seems normal for the conditions. But I'm worried now that packing it all in so close on a PCB will lead to unwanted noise.

I appreciate any input/advice about my layout or my circuit!

 

[danadakk]

Some useful material, ignore MPU base, the ap notes generic to mixed signal
work -

http://www.cypress.com/documentatio...soc-4-and-psoc-5lp-mixed-signal-circuit-board

http://hottconsultants.com/pdf_files/june2001pcd_mixedsignal.pdf

http://www.teledyne-e2v.com/content/uploads/2018/12/0999B_Board_Layout_AN.pdf

http://www.ti.com/lit/slyt512

Regards, Dana.

 

[hummusdude]

Ok, so these references are very helpful so thanks again for the links. I didn't find anything, however, related to my question about how far apart the analog and digital lines should be, or how to deal with analog signals that have to connect to digital components. There was some mention of partitioning a ground plane with a bridge and putting the mixed-signal component at that point, sort of a star ground idea. But as in the other sources I've been reading there seems to be a lot of agreement that when you do this it creates a dipole antenna effect with is not ideal. On my board I made sure to keep the analog and digital components grouped together. I have a solid ground plane on the bottom layer with the exception of some digital signal and power lines that jump to the bottom layer. By the look of it I'd say they are at most 2 or 3% of the bottom layer in total. For the signal lines that are on the bottom layer I tried to avoid long runs perpendicular to the general direction of the likely return current path so as to not force the return current to take a circuitous route back to ground.

One thing that did jump out at me was this statement regarding an ADC...

Separate power supplies for analog and digital circuits are also highly desirable, even if the voltages are the same. The analog supply should be used to power the converter. If the converter has a pin designated as a digital supply pin, it should be powered from a separate analog supply. All converter power pins should be decoupled to the analog ground plane, and all logic circuit power pins should be decoupled to the digital ground plane.

From this I get that I should power the dpot in my circuit from the analog side. Does that sound right?

 

[hummusdude]

Another question is regarding bypass caps for the digital components. I didn't add any...yet...in part because when bread boarded I didn't have any problems with noise disrupting the functioning of the digital controls. There is no ADC, high frequency or other very sensitive component to consider so even though it's generally advised I'm wondering if it's really that important for this kind of application.

 

[KlausST]

Hi,

To your questions:
1) The "free air distance" between analog and digital dies not matter much here.
* radiated noise won't care much about a mm more or less.
* coupled noise mainly travels via GND. Thus you need a good GND concept.
2) Is there a second question?

****
Ground concept is the key to a low noise audio circuit.
* you say

The board is 2-sided and the whole bottom is a ground plane.

.
When you have traces within a GND plane it is no GND plane anymore. Since it is cut into pieces it just is a lot of copper, but not much better than traces.
There are many discussions about GND planes (and "copper pour") here in the forum.

* one GND concept is " GND star point" wiring. In your case there are several sources of GND current: Two supplies, each audio input, each audio output.
True isolated designs are very difficult, thus one needs to connect these GNDs somehow. But when connected you can't control the (magnitude) of the GND currents. Switch mode wall warts will cause high frequency GND current, connected audio GNDs may cause GND loops, maybe resonance at some frequencies.
Thus having several GND connections (with big distance) on a PCB will cause GND current travel across the PCB. Even a true GND plane will cause voltage drop (audible noise) and coupled noise into signal traces...
Instead of keeping GND connections far apart, I'd rather put them close together to avoid GND currents across a wide area.
Better do all the GND connections on a separte star point - not on the PCB. Just feed one single GND to the PCB. Or feed two seperate GND (noise free for audio, "noisy" for power supply and digital part) wires to the PCB, but then these two GNDs must not be connected on the PCB. If you need to protect both GNDs from accidentally drifting apart, then use two anti parallel diodes to connect them. This limits the voltage difference to +/-0.6V.

* the dpot (control lines) could be easily isolated with optocouplers. Generate the dpot supply from the analog section supply.

* use bulk capacitors. Use fast ceramics decoupling capacitors at each supply pin of each IC/ module.

There is no single "correct" solution. All is "requirements" and the "compromise" to fulfill them.
Every designer has it's favourites. Several concepts, endless discussions....

Added:
About distance between analog and digital signals: Coupled noise not only depends on "distance" but also on "length" and "orientation".
Thus - wherever poissible - I feed noisy signals in 90° to the sensitive signals.

2 Layer: a low noise 2 layer concept is far more difficult and needs much more experience than on a 4 layer PCB. So don't be afraid of using 4 layers.

Klaus

 

[danadakk]

Not all caps are equal in bypass performance for the same value, pay
careful attention, read cap datasheet, assume nothing.

Regards, Dana.

 

[danadakk]

Attached is a seminar handbook from National, chapt 9 some experienced
layout recommendations. Although focused on switchers applicability still
good for general mixed signal layout.

Regards, Dana.