I'm not surprised, compiling and organizing this kind of information is a task that inflates in scope as you realize how much there is to explain.
Audio is an interesting case because ground plane return currents will transition from path of least resistance to path of least return inductance in the middle of the audio band, as dictated by the skin depth.
Ground planes are useful at RF for their self-organizing effect where the return current follows the signal path back to the source, as long as it can travel across the surface of a conductor as it will not penetrate any further than the skin depth at the signal frequency. Which is why we see ground planes with lots of small holes, to give skin currents a surface to follow to the opposite side of the plane. But this only works when the skin depth of the signal frequency is well above the plane thickness.
When the frequency is so low that return currents cannot follow signal currents in a ground plane (because the plane is thinner than the skin depth), it is more effective to force the return current to follow the signal current by using differential traces than it is to rely on the ground plane. The magnetic field radiated with a ground plane can actually be larger because the signal and return currents take different paths and form a loop.
So I see ground plane usage on audio circuits as being distinct from RF where the skin depth is well above the plane thickness. If we want to incorporate ground planes into audio circuits, we need to make sure the return current follows the signal current even at frequencies where the ground plane is ineffective (which is everything below at least 5KHz).
This was being discussed a while back but never quite got off the ground:
https://www.diyaudio.com/community/...orch-preamplifier-part-ii.146693/post-4002288https://www.diyaudio.com/community/...orch-preamplifier-part-ii.146693/post-4004058
Audio is an interesting case because ground plane return currents will transition from path of least resistance to path of least return inductance in the middle of the audio band, as dictated by the skin depth.
Ground planes are useful at RF for their self-organizing effect where the return current follows the signal path back to the source, as long as it can travel across the surface of a conductor as it will not penetrate any further than the skin depth at the signal frequency. Which is why we see ground planes with lots of small holes, to give skin currents a surface to follow to the opposite side of the plane. But this only works when the skin depth of the signal frequency is well above the plane thickness.
When the frequency is so low that return currents cannot follow signal currents in a ground plane (because the plane is thinner than the skin depth), it is more effective to force the return current to follow the signal current by using differential traces than it is to rely on the ground plane. The magnetic field radiated with a ground plane can actually be larger because the signal and return currents take different paths and form a loop.
So I see ground plane usage on audio circuits as being distinct from RF where the skin depth is well above the plane thickness. If we want to incorporate ground planes into audio circuits, we need to make sure the return current follows the signal current even at frequencies where the ground plane is ineffective (which is everything below at least 5KHz).
This was being discussed a while back but never quite got off the ground:
https://www.diyaudio.com/community/...orch-preamplifier-part-ii.146693/post-4002288https://www.diyaudio.com/community/...orch-preamplifier-part-ii.146693/post-4004058
We need more discussion on this topic, most of the pcb layout techniques apply to high speed digital design.
I've read numerous articles, forum posts etc etc with lots of conflicting information, summarised as such:
Further reading:
If you really want to go down a rabbit hole, try a google search "ground planes for audio pcb"
I've read numerous articles, forum posts etc etc with lots of conflicting information, summarised as such:
- Star ground is good
- Star ground is bad
- Ground pours are okay if layers are stitched together (2 sided pcb)
- A solid ground plane is required
- A 4 layer board is required
- A 2 layer board is good enough
- Ground planes are bad for high currents
- Ground planes are good for high currents
- Minimise loops
Further reading:
If you really want to go down a rabbit hole, try a google search "ground planes for audio pcb"
Last edited:
Analogue Audio PCB layout is the same as any analogue layout, same with digital.
Interesting to see its still going after so many years... 8, been a while, for me quite tumultuous, though still laying out PCB's!!!
I agree with using differential traces, but again these need to be balanced (same impedance etc.), again really a ground plane is best, if you have the required number of layers... Double sided boards can be a hassle and require careful placement.
Interesting to see its still going after so many years... 8, been a while, for me quite tumultuous, though still laying out PCB's!!!
The $64 question, at what point do you consider moving from a double side pcb with ground pours to a 4 layer pcb with ground and power planes ? See example pcb I'm working on, its 2 sided with ground pours (the input stage area is 75mm x 60mm). (I haven't stitched the layers together at this point). Makes you wonder the performance of single sided pcb's from amplifiers in the 1970's.
Last edited:
You know that by quantifying the sources and susceptibility to induction, and determining whether the change will provide a meaningful increase in performance. You can speculate, but without studying you can still produce a 4 layer board that sucks. Identify signal/return pairs, measure the loop area of their current loops, and find out which ones are closest which have the highest radiation or sensitivity. Because ground planes don't work on half of the audio band, a good ground plane layout will probably start out as a good 1 or 2-sided layout.
The thing about the ground plane is that for audio, it really doesn't solve many routing problems because relying on it for anything will leave half of the audio band unprotected. So often the best approach is just to make a sensible normal layout and then add a "zero signal reference plane" or ZSRP, which is a ground pour where the only currents flowing are magnetically induced currents. You do this either by connecting the ZSRP to one point only (a central ground node or an IO ground shell), or by connecting to the plane only through capacitors which ensure that only frequencies within the max skin depth of the plane are able to flow.
To use a ground plane as more than a ZSRP is not necessarily a way to improve performance as much as it is a way to reduce the layer count of the board, and this is something that needs to be done with understanding, and you don't achieve understanding without studying the current loops of your particular circuit.
The thing about the ground plane is that for audio, it really doesn't solve many routing problems because relying on it for anything will leave half of the audio band unprotected. So often the best approach is just to make a sensible normal layout and then add a "zero signal reference plane" or ZSRP, which is a ground pour where the only currents flowing are magnetically induced currents. You do this either by connecting the ZSRP to one point only (a central ground node or an IO ground shell), or by connecting to the plane only through capacitors which ensure that only frequencies within the max skin depth of the plane are able to flow.
To use a ground plane as more than a ZSRP is not necessarily a way to improve performance as much as it is a way to reduce the layer count of the board, and this is something that needs to be done with understanding, and you don't achieve understanding without studying the current loops of your particular circuit.
I'll add that it's entirely possible to add a ground plane without any meaningful increase in performance at audio, if your conditions aren't harsh enough or the layout is already really good. So it can be a wasted effort if you don't first identify exactly what you are trying to fix and whether a ground plane is the solution to your actual problems. If your problems are imaginary, then your performance improvements will also be imaginary. There are many good amplifiers which don't have ground planes. I would say that adding a ZSRP is the most likely way to add a ground plane to an existing layout without causing more problems if you don't want to think to hard. But since this is a hobby, most of us want to go beyond convenience.
Hi all,
Interesting to see that this subject is being picked up again ... Somehow my feel is that a good layout actually is the key to achieving results that are really good ...
As it is I have recently been trying to find more information about what may generally be considered superb audio related PCB layouts - sort of like reference layouts - with an accompanying description of why the layout was made the way it is. That is, why are components placed the way they are, why are tracks routed as they are (width, placement, what are the (important) current/return loops (magnitudes), which particular approach is considered to be the most important in achieving such good results in a particular layout, etc. Essentially, "what were the strokes of genius in this reference layout"
I suppose it could also be called "an analytical description of the process that led to the (outstanding) results of this PCB layout".
As keantoken mentions (I hope that I read your comments correctly) it appears to be the process of understanding the circuitry to be laid out that also in my thinking is key.
However, finding such information has been pretty tricky (i.e. mostly unsuccessful), but I have found some videos on youtube that go some way in addressing audio related PCB layouts. One of them (which I actually find to be really, really helpful) is this video with Rick Hartley who apparently has been an acknowledged PCB developer for decades:
To me there are myriads of tips on e.g. PCB grounding, current return paths (directly related to this discussion at 35:42, additional information prior to this time in the video), shielding, PCB stackup (not the usual signal-ground-power-signal), a different view of where the energy in a PCB exists (~close to the beginning), choice of decoupling capacitors (digital), mixed signal layout spacing, split GND planes & more. It is a lengthy video but, to me, well worth the time spent.
There is an additional video with Rick Hartley (interviewed by Robert Feranec) which e.g. discusses the challenges of splitting a GND plane, SMPS layout (25:58), input/output filtering, and connecting to a chassis:
Incidentally, Robert Feranec appears to have been exploring PCB layout (mainly digital) to some extent and has published many videos about this on youtube. I have only seen a couple of them but found this very useful in terms of showing why lining a digital trace with vias may be a (very) good idea (summary at 16:30):
@keantoken:
In general I would, as I mention above, be very interested in seeing examples of what are considered superb audio PCB layouts - particularly if such layouts are also accompanied with an analysis of why the various solutions on the board were chosen as they were. I would very much appreciate if someone knew of such information (videos or other media).
BTW - years ago marce directed me to this free tool which I have been using extensively since then e.g. for crosstalk assessments:
https://saturnpcb.com/saturn-pcb-toolkit/
And then a final thought in this post: If this subject is to take off might it then be an idea to start a new thread so as to be able to edit the first post with relevant links, new information etc.?
Cheers,
Jesper
Interesting to see that this subject is being picked up again ... Somehow my feel is that a good layout actually is the key to achieving results that are really good ...
As it is I have recently been trying to find more information about what may generally be considered superb audio related PCB layouts - sort of like reference layouts - with an accompanying description of why the layout was made the way it is. That is, why are components placed the way they are, why are tracks routed as they are (width, placement, what are the (important) current/return loops (magnitudes), which particular approach is considered to be the most important in achieving such good results in a particular layout, etc. Essentially, "what were the strokes of genius in this reference layout"
I suppose it could also be called "an analytical description of the process that led to the (outstanding) results of this PCB layout".
As keantoken mentions (I hope that I read your comments correctly) it appears to be the process of understanding the circuitry to be laid out that also in my thinking is key.
However, finding such information has been pretty tricky (i.e. mostly unsuccessful), but I have found some videos on youtube that go some way in addressing audio related PCB layouts. One of them (which I actually find to be really, really helpful) is this video with Rick Hartley who apparently has been an acknowledged PCB developer for decades:
To me there are myriads of tips on e.g. PCB grounding, current return paths (directly related to this discussion at 35:42, additional information prior to this time in the video), shielding, PCB stackup (not the usual signal-ground-power-signal), a different view of where the energy in a PCB exists (~close to the beginning), choice of decoupling capacitors (digital), mixed signal layout spacing, split GND planes & more. It is a lengthy video but, to me, well worth the time spent.
There is an additional video with Rick Hartley (interviewed by Robert Feranec) which e.g. discusses the challenges of splitting a GND plane, SMPS layout (25:58), input/output filtering, and connecting to a chassis:
Incidentally, Robert Feranec appears to have been exploring PCB layout (mainly digital) to some extent and has published many videos about this on youtube. I have only seen a couple of them but found this very useful in terms of showing why lining a digital trace with vias may be a (very) good idea (summary at 16:30):
@keantoken:
Any chance you have an example of how you use this in practice? A google search did not come up with anything that looked relevant ...
In general I would, as I mention above, be very interested in seeing examples of what are considered superb audio PCB layouts - particularly if such layouts are also accompanied with an analysis of why the various solutions on the board were chosen as they were. I would very much appreciate if someone knew of such information (videos or other media).
BTW - years ago marce directed me to this free tool which I have been using extensively since then e.g. for crosstalk assessments:
https://saturnpcb.com/saturn-pcb-toolkit/
And then a final thought in this post: If this subject is to take off might it then be an idea to start a new thread so as to be able to edit the first post with relevant links, new information etc.?
Cheers,
Jesper
Great post Jesper, this is a great summary.
I have been thinking along the same lines.
I was thinking of tackling this experimentally and with simulation.
For example, making a ground plane PCB and star ground PCB of the same nominal design. And actually measuring the performance of the amplifier.
I don’t have access to any fancy EM simulation tools, but I was talking to the creator or one, he was happy to run the simulation given that the results be published online for publicity.
I would be delighted to make it a group effort if other people want to join.
I was actually approaching this from a valve audio project perspective, so pure analogue.
I have been thinking along the same lines.
I was thinking of tackling this experimentally and with simulation.
For example, making a ground plane PCB and star ground PCB of the same nominal design. And actually measuring the performance of the amplifier.
I don’t have access to any fancy EM simulation tools, but I was talking to the creator or one, he was happy to run the simulation given that the results be published online for publicity.
I would be delighted to make it a group effort if other people want to join.
I was actually approaching this from a valve audio project perspective, so pure analogue.
Last edited by a moderator:
A few ideas that come to mind:
Prioritise track lengths. If they can't all be short, look at I/O resistances. For instance, an op-amp output with a 1M resistor: on the op-amp side the signal is strong, but on the receiving end (JFET base, NFB etc), which may be far away, the signal is much more susceptible to noise and RF so the resistor needs to be very close to the receiver.
Capacitors also act as voltage sources.
Differential voltages: ground planes are a bit of a cure-all, but tracks that are related by opposite signal polarity should usually be kept close together (same principle as twisted pairs and CAT-5 cabling etc).
Sometimes a scrunched up layout may help to reduce loop area, which helps to reduce parasitic inductance.
Thermal issues: ground planes can make things hard to solder, so use thermal relief 'spokes' where possible.
I find that ratsnests can be annoying if there is too much going on all at once. So I colour code things like power planes. Or they could even be temporarily made "no connection" in the schematic, to really help focus.
None of the EDAs I've seen allow you to separate "common" connections to 3 or more components into subcomponents, so you have to pay attention if you want a thin signal line hanging off a fat power line. Adding test points on the schematic level could helpful there.
Prioritise track lengths. If they can't all be short, look at I/O resistances. For instance, an op-amp output with a 1M resistor: on the op-amp side the signal is strong, but on the receiving end (JFET base, NFB etc), which may be far away, the signal is much more susceptible to noise and RF so the resistor needs to be very close to the receiver.
Capacitors also act as voltage sources.
Differential voltages: ground planes are a bit of a cure-all, but tracks that are related by opposite signal polarity should usually be kept close together (same principle as twisted pairs and CAT-5 cabling etc).
Sometimes a scrunched up layout may help to reduce loop area, which helps to reduce parasitic inductance.
Thermal issues: ground planes can make things hard to solder, so use thermal relief 'spokes' where possible.
I find that ratsnests can be annoying if there is too much going on all at once. So I colour code things like power planes. Or they could even be temporarily made "no connection" in the schematic, to really help focus.
None of the EDAs I've seen allow you to separate "common" connections to 3 or more components into subcomponents, so you have to pay attention if you want a thin signal line hanging off a fat power line. Adding test points on the schematic level could helpful there.
Yes, good points, the basis of the art of engineering.
True, DC to about 5khz or so is mostly resisistive and beyond is reactive. I see this in pcb layouts where the ground plane is routed to control return currents. Probably another reason why copper pours are used on the top layers.
I've not found much information on this apart from being referenced as stitching via capacitors where pcb tracks cross split ground planes.
It's difficult to consider what is a "reference layout", as Keantoken has pointed out it depends on the design goals and/or the engineering analysis. Here is an example, would you use a 4 layer pcb for a cheap $100 consumer product with modest design criterea, not really, it's too expensive and there would be little benefit in performance considering the cost of the product. Would you a 4 layer pcb for a industrial product that costs $5000 and has to meet certain international standards, well yes, when you consider the engineering and development costs it makes sense to use a multilayer pcb to meet the design goals and criteria.
This is probably the definition of Engineering.
I also find Robert's videos very educational.
I'm not sure splitting this thread into a new one is such a good idea, I would probably say this is probably the best thread to accumulate general knowledge for pcb layout guideline and techniques.
Star grounds are no longer used in pcb design in a traditional methodology, Here is a article from Altium- Should you use a star ground for mixed signal grounding.
Here is a nice tool to visualise your gerbers in 3D - ZOFZPCB Gerber 3D Viewer.
The user interface is a little quirky, once you find your way around it works quite well.
The user interface is a little quirky, once you find your way around it works quite well.
Jesper, I forgot to add this to my other reply, this is exactly what I did when I started laying out my pcb, looking at other amplifier layouts, only to realise that I needed to understand the reasoning behind the pcb design as Keantoken pointed out in posts #106 and #107.
There can be a number of factors that determine the design of a pcb, the end cost of a product, engineering analysis, meeting EMI standards or physical size or shape of a product. It could be the case that compromises may need to be made somewhere in the product design phase and processes. It can be difficult to understand a pcb layout for a audio amplifier without having the knowledge from the engineers as to how or why they arrived at a particular design.
If we do nothing else, we should at least start with good engineering practice such as understanding current flows in a circuit and the associated return paths. I'm sure that most of us, myself included, find this concept the most difficult to visualise in complex circuits such as audio power amplifiers where you have both AC and DC low and high currents circulating on the same pcb. As you have seen in the Robert Feranecs videos, the professionals have nice EM simulation tools to assist them with their pcb layouts.
Thanks, I will read in a bit more depth later, seems a good article.
This seems to be the crucial point:
I’m trying to get this point clear.
Are they assuming a hybrid scheme; star ground and ground plane? Can someone sketch what they mean by “the second you route across a gap in your ground regions”?
A few diagrams would make that article better.
I agree, a picture is worth a thousand words when trying to visualise these types of concepts.
Try these links, hopefully the images provide a better idea of the concept.
Try these links, hopefully the images provide a better idea of the concept.
- Staying Well Grounded
- learnemc.com/pcb-layout - See figures 6, 7, 8 and 9
- Hottconsultants - mixed signal pcb - opens in pdf
- elmac.co.uk -EMC_SelfStudy- power and ground planes
@boyfarrell:
Actually, in one of the Rick Hartley videos I linked to above there's a very clear reference to this. He shows results from a Japanese study (I think it was) where the consequences of routing across a gap in a ground plane is shown (appr. 43:42 in the how to achieve proper ground ... video).
Have you any idea about what the strengths or shortcomings of this EM simulation tool is? Can it do mixed-signal, analog and digital simulations? Does it have all the simulation files available, or ... ? Essentially, do you know which information is needed to have him make such a simulation?
@Indiglo:
One example of this could be Robert Feranec's via simulation video (linked to above) where henceforth I will simply line digital traces with vias on both sides of the trace - and likely will also do this with analog traces in order to ground the higher audio frequencies so that they do not spread out (as much) on the PCB (the lower frequencies are less insisting on creating crosstalk). One question to clarify in this context, though, is how much such a trace via lining changes the impedance of the trace surrounded by the vias ...
Another could be an LTC2380-24 ADC layout I have been working on for some time now where I achieved a ~ 10 dB better 2H etc. THD figure by changing a small layout detail that was implemented in Linear's demoboard of this ADC. The trick simply was to route the OVdd trace on the inside of the adjacent GND pin. In effect this small trick probably acts like a guard ring isolating data transmission GND noise from the other parts of the ADC. A puzzling approach though because the data transmission only is active when the ADC is not sampling - but the results were quite clear. And this was not something that I would have thought of myself (or, if I had I also prefer not to make 10 different PCB designs so such tips are really welcome).
However, with this in mind, I remain very interested in seeing/reading about reference PCB layouts/"flashes of PCB layout genius". Outside of a hopefully generally good knowledge of PCB layout theory my feel is that such reference layouts may be practical examples of how such theory may be best implemented in practice.
Anyway, the day is approaching - cheers,
Jesper
Firstly, I have not read the article but I guess what they mean is that when there is a gap in a "ground connection" the return currents, i.e. the current flowing in the ground(s) need to go around the gap. And, depending on the frequencies present in these return currents, this "going around" may either be relatively smooth (like folding around the gap if lower frequencies), or spreading out as noise signals if the return currents contain higher frequencies.
Actually, in one of the Rick Hartley videos I linked to above there's a very clear reference to this. He shows results from a Japanese study (I think it was) where the consequences of routing across a gap in a ground plane is shown (appr. 43:42 in the how to achieve proper ground ... video).
If that is actually an option it could be quite interesting to do this
Have you any idea about what the strengths or shortcomings of this EM simulation tool is? Can it do mixed-signal, analog and digital simulations? Does it have all the simulation files available, or ... ? Essentially, do you know which information is needed to have him make such a simulation?@Indiglo:
To me the thing is that I learn a lot from either reading or seeing how other people have solved particular "challenges". And if the criteria for a given PCB layout analysis, or solution, is given initially or during the analysis, it may often be very helpful to me anyway. It is like picking up "bits and pieces" here and there and in this process clarify my own approaches to PCB layout.
One example of this could be Robert Feranec's via simulation video (linked to above) where henceforth I will simply line digital traces with vias on both sides of the trace - and likely will also do this with analog traces in order to ground the higher audio frequencies so that they do not spread out (as much) on the PCB (the lower frequencies are less insisting on creating crosstalk). One question to clarify in this context, though, is how much such a trace via lining changes the impedance of the trace surrounded by the vias ...
Another could be an LTC2380-24 ADC layout I have been working on for some time now where I achieved a ~ 10 dB better 2H etc. THD figure by changing a small layout detail that was implemented in Linear's demoboard of this ADC. The trick simply was to route the OVdd trace on the inside of the adjacent GND pin. In effect this small trick probably acts like a guard ring isolating data transmission GND noise from the other parts of the ADC. A puzzling approach though because the data transmission only is active when the ADC is not sampling - but the results were quite clear. And this was not something that I would have thought of myself (or, if I had I also prefer not to make 10 different PCB designs so such tips are really welcome).
However, with this in mind, I remain very interested in seeing/reading about reference PCB layouts/"flashes of PCB layout genius". Outside of a hopefully generally good knowledge of PCB layout theory my feel is that such reference layouts may be practical examples of how such theory may be best implemented in practice.
BTW: In your layout design above - have you considered making the board a "2½ layer" design? By this I mean keeping a quite contiguous GND plane and then routing wires on the bottom side to the places where this is unavoidable? It is my impression that if the wires are kept close to the GND plane - and it is audio frequencies - then this may be a cost effective way to "increase" the layer count of the board. Just a thought ...
My thought here is that this thread was started in 2013, and the OP might not be that active anymore so that gathering relevant information in post #1 (for all to easily access) may no longer be an option ...
Anyway, the day is approaching - cheers,
Jesper
Last edited:
All very good points, I have learnt many things along the way from other peoples designs when laying out my pcb and I'm still tying to understand all the return current paths, made all the more complicated by the fact I have added to the design +/-15vdc and +/-50vdc regulated supply rails.
Yes I have, it's the 3rd attempt at the layout. I got part way through the first two layouts only to come to the conclusion that it didn't quiet look right. It's a fairly tight layout, most of the tracks are on the top layer and where I couldn't route was put on the bottom layer and used ground pours on both layers, probably not ideal and I have to move the DC power supply inputs because the ground pours are obstructed for the return currents. I can change to a 4 layer board if required without changing the component layout and this will give me a proper ground plane to work from. The next challenge is the driver and output stages and how to route the high current return ground tracks, this is where sometimes looking at other power amplifier layouts can help.
BTW, the amplifier is a slightly modified version of this circuit from this thread - Slewmaster - CFA vs. VFA "Rumble"
The difficulties laying out this circuit arises from the push pull differential input stage because you have tracks crossing over from the edges of the pcb to the centre. As seen from the bottom image in my post #105
Yes I have, it's the 3rd attempt at the layout. I got part way through the first two layouts only to come to the conclusion that it didn't quiet look right. It's a fairly tight layout, most of the tracks are on the top layer and where I couldn't route was put on the bottom layer and used ground pours on both layers, probably not ideal and I have to move the DC power supply inputs because the ground pours are obstructed for the return currents. I can change to a 4 layer board if required without changing the component layout and this will give me a proper ground plane to work from. The next challenge is the driver and output stages and how to route the high current return ground tracks, this is where sometimes looking at other power amplifier layouts can help.
BTW, the amplifier is a slightly modified version of this circuit from this thread - Slewmaster - CFA vs. VFA "Rumble"
The difficulties laying out this circuit arises from the push pull differential input stage because you have tracks crossing over from the edges of the pcb to the centre. As seen from the bottom image in my post #105