I have completed a 2-layer layout for a low voltage audio design that uses dual rail 15V DC power (15-0-15) at low current (<350mA per rail). Front layer features all audio signal and power tracks, and the back layer features 0V ground pours where required. I class myself as a hobbyist of 40+ years, and certainly not an engineer beyond basic theory understanding.
My question relates to running low current low voltage DC tracks above sections of the 0V ground pour. At these levels of low current consumption, is my routing critical or ‘storm in a teacup’ thinking? I have observed other designs where DC rails are kept clear of 0V pours.
Important to note that all signal-related ground pours are entirely separate to the power’s 0V GND (not shown in the screeen below).
Within the area of the board related to the on-board PSU (LM317T, LM337T and associated components), there are plenty of instances where the 15V rails pass above the 0V pour in that region. So if tracks traverse above the 0v pour in that region, then the same issue occuring per the screenshot, is likely a non event?
Your design and what you write looks like you are trying to avoid having GND pour under your tracks when it is absolutely opposite. Each current (supply or signal) flows in closed circuit. For most currents at PCB the back to source way is through GND pour. The smaller the area surrounded by a circuit the better - any current changes in circuit generates smaller magnetic field changes and as small as possible of any external magnetic field is flowing through your circuit generating unneeded fluctuations in it.
If each track has continuous GND pour under it then the area of circuit is the smallest (not 0 as PCB thickness is not 0).
Nowadays when we live in lots of strong magnetic fields everywhere (cell phones) this is more important than 40 years ago. The ways of designing PCBs that were good those times are no longer good.
I don’t design audio circuits so can’t say anything ‘for sure’ but you certainly should not avoid going with track over GND zone on the other PCB side.
Here is an example of my 2 layer (digital) PCB:
The idea behind it was to have continuous GND behind each track.
I agree with the above here. For DC (and proper decoupling at both ends) it does not matter much. Except for EMC. Bigger loop areas both emit and pick up more EMC, and the tighter the coupling is between the GND plane and any other signal (including power) the better it is. A bit of distributed capacitance under your power tracks may even help a bit with filtering out EMC / noise, (but it more likely acts as a transmission line and just feed the noise through to the other end).
The main thing is how to manage the currents flowing though the GND plane. If you have an SMPS on the left, and a stepper motor controller on the right, then don’t put your sensitive microphone amplifier in the center of the board. Rick Harley has made an excellent 2 hour and 19 minute video presentation about GND planes and how currents propagate though them. It’s mostly geared towards digital design, but the same principles are true for analog stuff.
@Piotr@paulvdh Guys, thank you for the detailed responses. I appreciate this very much. The design is a duplication of a 1981 design where a single layer board was used. I’ve replicated the component layout and attempted to maintain the same copper trace routes per the original 1981 layout. The only difference is the PSU on the left of the board, which is not original.
Are you suggesting that the 0V pour should (or could) encompass the entire board (with my exception of the three isolated signal grounds of course)?
There is so much conflicting information around, I have found statements that support wholesale ground pours, and others that suggest to “go easy on the pours”, et-al.
I am also lacking detailed knowledge concerning analog PCB design. One thing you get with a big GND plane is capacitive coupling to that GND plane. This can be minimized by using thinner tracks, but at audio frequencies this is not a big issue. Note that even a 0.25mm narrow track can already handle over 500mA, but you will start to get some loss due to the copper resistance.
Another factor I’ve heard a lot and seems plausible is that PCB’s may get bent during production if there is a big difference between the amount of copper on the top and bottom sides, but apparently that was in years gone by a lot bigger issue then in the modern world.
To add to your confusion here you can find in my opinion the best articles I have ever read about PCB design:
I want to remind you once more - when this PCB was designed the designer assumed 0 cellphones working in the immediate vicinity of the device.
I don’t understand what you are saying.
If the original was single layer and you tried to maintain the same copper trace routes you should have single layer PCB while you have two layer.
I am referring to the year 1981, the design was published in a local electronics magazine, and eventually sold as a kit from local electronics retailers here in Australia.
I switched from the board’s original 1-layer design to 2-layer based on feedback I received when I started this ‘copy’ project, suggesting a 2-layer board with relevant ground planes.
Also, the revised power supply section (which is significantly more complex than the original circuit) functions best as 2-layer due to component placement, etc.
Here’s a screen of the original board layout from 43 years back.
In an audio circuit (I assume some sort of pre-amp) the goals is to keep different channels from coupling from one channel to the other. Assuming you have more than one channel. It is usually wise to keep two channels “balanced” in that these two channel clad should be a mirror of the other channel.
You will also need for capacitors, some for bulk energy and some for high frequency, these would be for the power supplies.
What changes would you make to the 0V pour? @Piotr shared reams of information on the subject, I’ll start sifting through it all, but beyond attempting to replicate the original layout, I’m kind of flying blind until such time as I digest all the info shared. I am pouring over a Douglas Self book also (Small Signal Audio design) which is fairly easy to take in!
For the record, the original design sounds phenomenal when set up. Its specs are solid, hence the interest in the design. The designer is highly revered. I suspect that if he had his time over, he may invest in a 2 or 4 layer board, using ground planes more effectively. Who knows.
Im no Expert but i stumbled across a video discussing these ideas, like star grounding, seperate grounds and that they usually are actually counter productive.
I have designed quite a few simple audio boards, most were analogue only, so whilst the incoming supply was +5v, I used an isolated DC:DC converter, and kept the Gnds separate. I have 2 boards that also needed some logic, so had 2 separate grounds.
In one case, I kept the small amount of logic to one side of the board, the analogue to the other, with the only “linkage” between the two being a relay… so nicely isolated: this used 4 ground zones: a pair of digital grounds on one side, a pair of analogue grounds the other. However, I also added some adjacent THP holes, so that I had the option to connect the two grounds, if I wanted / needed to.
The other was a silence detector, far more complicated, so I was unable to separate the grounds at all, so just combined the incoming 5v’s ground to the analogue ground (DC:DC converter again). The main audio through-path was passive, but I had to take a capacitively coupled high-impedance “sniff” of the incoming audio. I guess, because it was a fairly simple circuit, there were no ground issues at all. The tracks were two sided, and I just ground filled all that was left on both sides.
@InsaneDruid thanks for sharing the video. Hans Rosenberg has a great way to present often complex subjects - perfect for me!
With regards to my preamplifier redux, there are a number of audio signal grounds that the designer, Dr. David Tilbrook, used. I will watch more of Hans’ videos to try to better understand how Tilbrook’s approach either aligns or works in contrast.
As others here have rightfully argued, mobile phones and wi-fi were yet to be invented in the early 80s!
Gosh, and to think that I was close to ordering boards…
@vintage It’s pretty much off topic, but I think you’ll like it.
Tonto is one of the early synthesizers from the’70-ies, and hit had quite severe EMI problems, you could not use it while a computer was switched on nearby, and at some time (around 18 minutes into the video) they put in a mesh of copper pipes to screen out interference from radio stations.
I did EMC and Signal Integrity design for almost 20 years and my designs performed extremely well. I served on ANSI, CISPR, and helped with FCC specifications.
I wish i could give you a beautiful single line answer, but low frequency analog and digital or RF are two entirely different animals. Digital signals that coupled into the analog section could hardly be seen on a scope, but were readily audible when played through a speaker. The audio ground and the digital areas needed careful isolation.
Fortunately, it sounds like you are using linear power devices, which solves that part of the problem. Your power supplies should all be happy to be referenced to your analog signals.
You’ve gotten some great advice about the area fills (you call “pours”). Good coupling to the ground fills are desirable as long as you don’t have mixed signal types. As one person mentioned, BOARD WARPAGE IS YOUR ENEMY. You can help this by crosshatching the ground fill, putting trace connections, or pairing it with another filled plane exactly equal and opposite to the middle of the board (i.e. top - 5mil dielectric- ground (or power) plane - 50 mile dielectric - Power (or ground) plane - 5 mil dielectric - bottom trace). This gives a 57 Ohm board when using affordable 6 mile traces.
Your frequencies are so low that you don’t have to worry about impedance or trace edges.
1950’s boards were also done on different materials (as well as rarely having planes). The FR4 we use today (or whatever new version) is susceptible to warping.
