4 layer PCB arrangement with multiple power layers

[MNMNMNMN]

Hi, after long lurking I'm proud to make my first post.

I work as a repairman for electronic musical instruments, mainly, and do some occasional design as well. In the Eurorack Modular world (started by Dieter Doepfer http://www.doepfer.de/home_e.htm ) we use +12V, -12V, and a 5V rail, mainly for digital modules. Power can come from either a linear PSU or a Switched PSU. In standard DIN-rails we can mount a plethora of different modules ranging from simple analog Oscillators to complex digital effects and sound sources. Tons of manufacturers, big and small, from all over the world design modules: Like these.

To power all these modules we use a (what we call) bus board.
 

You can see the 4 power rails, 5V, +12V, GND and -12V, accompanied by a LED to show there is power. Modules connect via IDC connectors, either 10 or 16 pins. There are 2 more traces, GATE and CV. (some modules use these traces for all sort of voltages, ranging from digital syncs, to pitch information for the Oscillators.) Gate is a trigger signal from 0V to 10V, and CV is Control Voltage from -10V to +10V. The CV can not drift, or experience a voltage change, because that would make the music out of tune.

Now for the question: I want to design my own bus board in a ultra flat profile (because there is non yet). I want to use a 4 layer PCB, and have dedicated planes for the power rails and GND. The CV and GATE trace needs to share the PCB with a power rail. What is the best practice to sandwich these layers?  Where should I place the GND-plane? And is it best to place the CV and GATE traces on the GND-layer?

I understand there is a capacative effect when we sandwich power layers. This could be beneficial for smoothing out voltages, but how should I layer the + and - rails? The GND in between, or should I keep the + and - rail on top of each other? Does it even matter?
My knowledge is lacking (for now) to make any meaningful measurements, as is my equipment I think.
Manufacturers use quite wide traces on 2-layer PCB's these days, but the Amperage can become quite significant and cause drops on the far ends of the bus board. A lot of people consider this bad design and think it's time for improvement.

I'm curious to see your guys' thoughts and what I might be missing! 

[srce]

Every once in a while there pops up a PCB stackup question, and you can search the forum to find previous answers.

Put it simple, so whatever you like.

There are a few common stackups, mostly SPPS or SPSP, where S is signal, P is power or ground.

Isn't this more a question of what to do when you have more than 2 power rails on a 4-layer PCB? You can't have "dedicated planes" if there are more rails than layers. You need split planes, right?

[T3sl4co1l]

Don't worry about it. You aren't doing any signal quality stuff in that kind of system, and the backplane doesn't need to be particularly robust, you'll be using local bypass on the cards after all, right?  Two layers, routed power, poured ground, will be more than enough.

Tim

[nigelwright7557]

There is little capacitance between planes.
The main advantage of a power plane is the virtually zero ohm resistance in it.
The circuit should be properly decoupled anyway.

[Yansi]

Aint +-10V signal levels with just +-12V supply voltage  kind of on the dumb side? Requires to push the opamps way to close to the output limits.

[MNMNMNMN]

[...] you'll be using local bypass on the cards after all, right?  Two layers, routed power, poured ground, will be more than enough.

Yes, pretty much all modules have local bypass where the power enters the module. It is also a bad design (according to some) to use IDC, with their very small gauge wires. But that's another question. Some Indie developers started a movement with backwards compatible thick gauge connectors.

Aint +-10V signal levels with just +-12V supply voltage  kind of on the dumb side?

Yes, it would seem so, but this has been the case for several decades. In practice most control voltages range from +5V to -5V, or 0V to +/-10V. But let's not get into further design practices in the synthesizer world. (for now )

There is little capacitance between planes.
The main advantage of a power plane is the virtually zero ohm resistance in it.

Okay, capacitance is negligible in this scenario as it seems. But the lowest resistance possible is actually my motivation to prevent voltage drop across the bus board. Hence why big pour planes. If I'm not mistaken I should be able to calculate a potential drop am I not?

You aren't doing any signal quality stuff in that kind of system, [...]

Well, it seems like we are. Interference from digital modules is audible on voltage controlled amplifiers in some scenarios, just like OLED displays. But if I understand correct, that has nothing to do with the bus board, but more with bypassing? Somehow, some modules do 'inject' some sort of noise in the system, whether it be the power rails, or something else.

Isn't this more a question of what to do when you have more than 2 power rails on a 4-layer PCB? You can't have "dedicated planes" if there are more rails than layers. You need split planes, right?

Yes, but what is considered best practice when it comes to the arrangement of +V to GND to -V. Should I separate the + and - rails with a GND plane, or not?

If I were you, I would go with SPSP, with first layer being your signals, second layer being a ground layer, third layer being power, and last layer being another ground.

That leaves me with a power rail left, or would you combine +12V and -12V on the same layer? Otherwise I need a six layer board, and that's even more overkill.


I mainly got inspired by this man: http://www.hinton-instruments.co.uk/paprod/psu/distribution.htm who seems to spare no expense regarding power supplies and distribution. Thick aluminum bars to keep resistance to a minimum. And besides that, also takes proper grounding/earthing not as a afterthought, like most manufacturers seem to do. (No grounding at all!)

Aint +-10V signal levels with just +-12V supply voltage  kind of on the dumb side? Requires to push the opamps way to close to the output limits.

OPA1612 has -120 dB or less THD at 2V margin, and that's limited by input, not output. With higher gain, OPA1612 has -140dB THD at 1V margin.

For critical parts of the circuit we very often see OPA's, when it is less critical we mainly use TL0xx's.

You guys have already given me a lot of food for thought, thanks!

[MNMNMNMN]

It's just better to forget about stackups and just use one layer for signal (preferably top), one layer for power, put the rails in parallel on one layer, and two ground layers to isolate signal and power from polluting each other.

Intuitively this seems like a good approach, but it wouldn't be my first time where my intuition has nothing to do with the reality

[MNMNMNMN]

Just to wrap it up: is having a +12V, a -12V and +5V rail on the same layer not going to cause interference between the rails? Separating the signals with a GND layer makes complete sense, but is there any benefit if I for example take the -12V layer as a separate layer?

[MNMNMNMN]

FYI, you are thinking way too much than what your application requires. Just make sure they connect, and all will be fine.

I like it like that But I try to do the things proper and want to make sure there is nothing more to gain.
I've seen Dave mention ground loops every now and then, would I not introduce several ground loops when I split the GND over more than one plane, and than also use a thick trace on yet another layer? I understand that if I connect the grounds on as many points as possible, using vias for example, this becomes less of an issue, but decent grounding is very important in audio.

[MNMNMNMN]

Yeah, that makes sense. In a modular synth there are indeed a lot of front panel connections, each carrying GND. What I understood earlier was, that by making a very low impedance path for the return current closest to the source (PSU), most of the current would travel there, and steer away from any signal lines. (this is my uneducated understanding of course) And since GND can be considered a power rail, not only signal lines benefit from low impedance and resistance traces, because the GND in audio systems have a big impact on audio quality (noise).


Well, I have a better vision of how to implement this, thanks everyone! 

[T3sl4co1l]

Well, it seems like we are. Interference from digital modules is audible on voltage controlled amplifiers in some scenarios, just like OLED displays. But if I understand correct, that has nothing to do with the bus board, but more with bypassing? Somehow, some modules do 'inject' some sort of noise in the system, whether it be the power rails, or something else.

You've got some kind of minefield here, with no standards or qualification process (I assume; this is all amateur, I take it?), spaghetti literally hanging off the front, and boards doing whatever it is they do.

I don't see signals on the backplane pictured, so I don't know how much you could expect to gain, regardless of its layout.  Grounding through the module rails or front panel would seem much more important, when high speed digital signals are distributed; even more important still, are the control of signal quality at digital sources and sinks, the use of appropriate cabling where possible, and the rejection of interference on all connections.

So, in short, it's up to each module.

The way commercial equipment is made, is testing it against a relatively high level of interference of different types, and measuring its emissions against a relatively low level.  Typical levels are 3V conducted in on cables, 3V/m radiated through space, and short transients of a few thousand volts in various ways (conducted and radiated; EFT and ESD).  Conversely the emissions are limited to a few mV, give or take (actual peaks can be 10s of mV if infrequent or modulated erratically, but it's averaged a bit due to how it's measured).  It should be very difficult indeed for properly functioning equipment to interfere with each other with this ~60dB margin between emissions and susceptibility!

This still works for modular components.  Computer cards have to meet approvals, on a somewhat different standard, but the idea is much the same.  A similar approach would be prudent in the design of your synth boards; but, good luck getting that done comprehensively.

I suppose one could make a test fixture, plug in a module and subject it to noise sources, and subjectively evaluate whether it's functional or not.  I'm not sure that such a fixture would be all that easy to use, or cheap to make or distribute; and there's always the problem that different people have different subjective thresholds for performance (or the tester can always outright lie).

So, I don't know that you can have a comprehensive and reliable test that the community can use, on an amateur budget.  You can of course make your own modules to your own standards, but for everyone else?  Best practices, is about it...

Tim

[MNMNMNMN]

And that is indeed what can be seen in the Eurorack world: A best practice. There are indeed a lot of (semi)-amateurs making modules, but also pretty big companies, like Roland or Behringer. Then there is Mutable Instruments (https://mutable-instruments.net/), a solo developer for hardware and firmware, but from his modules you can tell the scene is getting more serious since all his new modules are compliant with interference regulations and ROHS for example.

But yeah, all in all, it is a Wild West of 'standards' and best practices. I can safely conclude that my worries are not all that important I guess. That doesn't mean I shouldn't challenge myself to improve here and there, because in my daily routine of music production I do notice grounding issues, noise, impedance mismatch, audible LEDS on the other side of a system, strange fluctuations in pitch and other random glitches. The source of these problems, however, can be a lot of things, and a over-designed bus board might not be the solution. 

[MagicSmoker]

If you have digital stuff interfering with analog stuff that probably isn't something that can be fixed with the backplane. Adding Pi filters on all of the power rails in between each card connector might help reduce noise some, but the main effort should be focused on the cards themselves.

Consequently, this doesn't sound like it would really benefit from a 4-layer board, but if you subscribe to the, "better safe than sorry," philosophy then a good routing strategy for a 4-layer board is to dedicate one of the middle layers to ground then place all the power rails on the single layer to one side of the ground plane and all the signal traces on the remaining two layers on the other side of the ground plane (e.g. - Power - Ground - Signal - Signal).

If all of the signal and power rails can be routed more or less straight across the pin header connectors then a good 2-layer routing strategy would be to make the bottom layer a ground plane and route all the signal/power traces on the top layer.

EDIT - grammar

[langwadt]

I mainly got inspired by this man: http://www.hinton-instruments.co.uk/paprod/psu/distribution.htm who seems to spare no expense regarding power supplies and distribution. Thick aluminum bars to keep resistance to a minimum. And besides that, also takes proper grounding/earthing not as a afterthought, like most manufacturers seem to do. (No grounding at all!)

that just looks silly, does he also wire his house with 100^2mm wire and run water in 10" pipes?

[T3sl4co1l]

I'd make a joke comparing the embarrassing power consumption of analog versus digital circuitry, but really, audiophoolery is an adequate explanation I would think.

Tim

[MNMNMNMN]

[...]
If all of the signal and power rails can be routed more or less straight across the pin header connectors then a good 2-layer routing strategy would be to make the bottom layer a ground plane and route all the signal/power traces on the top layer.

Yes, this is possible, although to my surprise most bus boards do not even pour the ground layer. Some manufacturers do incorporate bypassing next to each connector but isn't that a bad idea if you don't know the consumption of the connected module?

I mainly got inspired by this man: http://www.hinton-instruments.co.uk/paprod/psu/distribution.htm who seems to spare no expense regarding power supplies and distribution. Thick aluminum bars to keep resistance to a minimum. And besides that, also takes proper grounding/earthing not as a afterthought, like most manufacturers seem to do. (No grounding at all!)

that just looks silly, does he also wire his house with 100^2mm wire and run water in 10" pipes?

I agree it does look like overkill, but I'm a little hesitant to discard his ideas. Hinton is a respected studio technician by enthusiasts and critics alike. When you make music, it are the little things that matter in the end. This is not a hifi-installation in a living room. I have here Neumann 3-way speakers, with a serious price tag, in a treated (acoustic) studio, and when you have a situation like that, other things suddenly become clear: noise way below the noise floor of a normal listening situation, but in the process of producing and mastering these small differences become important. By making absolutely sure you have done everything one could, you clear a path for a creative process, which in the end making music is. And yes, there is a lot of hocus pocus, but even the effect of psycho acoustics matter.

I'd make a joke comparing the embarrassing power consumption of analog versus digital circuitry, but really, audiophoolery is an adequate explanation I would think.

Tim

Now I'm curious about the joke  Perhaps we can conclude we can look at these designs from two perspectives? From a electronic engineering point of view, these small difference and the extra price tag are not justifiable, maybe. But when music production comes in, perhaps things change. I think most will agree that a Keysight or Tectronik has better specs than a Rigol, but the importance of those features only become important in the right use case, am I right?

[MagicSmoker]

Yes, this is possible, although to my surprise most bus boards do not even pour the ground layer. Some manufacturers do incorporate bypassing next to each connector but isn't that a bad idea if you don't know the consumption of the connected module?

Plain old capacitor bypassing for each supply voltage at each pin header/card connector is never a bad idea, though be wary of inadvertently creating an LC pulse shaping network or ladder filter if you only use SMT ceramic capacitors. Placing a few aluminum electrolytics every couple of card connectors (or 4-10cm) will dampen out any tendency towards oscillation/resonance due to their relatively high ESR.

[LoveLaika]

Isn't this more a question of what to do when you have more than 2 power rails on a 4-layer PCB? You can't have "dedicated planes" if there are more rails than layers. You need split planes, right?

Apparently I didn't bother to read the whole OP post .

And to answer that, it doesn't matter. For a typical 1.6mm 7628 stackup, you have 0.2mm between top and mid 1, 0.2mm between mid 2 and bottom, and the rest between mid 1 and mid 2, ignoring copper thickness.

For every 1cm2, you get 20pf of capacitance, which is nothing. For a 10cm*1cm copper bar, that's only 200pf, hardly anything for low frequency.



It's just better to forget about stackups and just use one layer for signal (preferably top), one layer for power, put the rails in parallel on one layer, and two ground layers to isolate signal and power from polluting each other.

I'm not OP, but I'm curious about the SPSP stackup. If you have 2 power inputs, then with SPSP, you can use the two planes and dedicate them to the inputs respectively as a plane. However, with more than 2 power inputs, what if you run traces within the inner layer and dedicate the last layer to Ground? In that sense, the inner P layer only routes power, but you don't have it as a plane specifically, just use that layer exclusively for power traces? If you do it like that, does that defeat the purpose of the stackup? In doing that, would it be better to have all layers be connected to ground? You can still run traces on ground planes, though doing so would disrupt the plane, but if you can't dedicate a plane like that to power with a plane, can you do it like this?