Planes, layers, ground, power, and two-sided PCBs

[GGBB]

I've been putting a ground plane along with most of the traces in the bottom layer of my double-sided PCBs. I keep power and bias supply traces in the top layer. I had also been using a power plane on the top side, and I never had any problems with this, but read somewhere that it's not a great idea for a couple of reasons, so lately I've omitted the plane on the top side.

Recently I've been reading and saw a couple of posts from RG which mentioned that ground planes are not really helpful for audio. He generally seems to discourage it unless there is very good reason. Now, I mainly use them because it makes ground routing a breeze, but it dawned on me that without a plane on the top layer, I could put grounds there and probably still have easy routing.

Convention in DIY fx pedal world seems to be ground planes - but convention isn't necessarily best practice.

So would it be a mistake to have ground and power/bias in the top layer and everything else in the bottom and have no planes? If so what problems does it introduce? Is anybody doing this?

[Kevin Mitchell]

I'm curious about this too. As far as my current knowledge goes, I thought it's only an issue with paths holding high frequency signals causing "cross talk" due to capacitance in the PCB material. We don't want artifacts of HF signals in our supply routes or anywhere else really.

I had asked about cross talk on another forum. I think it may be relevant to your post but honestly, we don't deal with HF signals often in the stomp box world.

What is crosstalk? (what is it and what causes it?)
It's when the characteristics of an oscillating signal show up on parallel signal - in this case we're taking about circuit board tracks (both next to and beneath). Parallel tracks act as a capacitor and capacitors pass/conduct higher frequencies easier than lower. The longer these tracks run parallel, the more capacitance & vulnerability they have. The main factors for crosstalk potential are the frequency of the signal, copper volume of the tracks, space between the tracks and also PCB material.

Is it a common issue with layouts? (do people combat crosstalk with new designs often?)
It is clear that this is a potential issue with higher frequencies. So it would depend on the design. I can imagine this being a factor when routing clock and data signals. Though not as crucial with VCO outputs, it's worth taking the necessary precautions to avoid any artifacts in the audio signal when playing higher octave notes. So I'd like to say no - as we would probably see more inquiries about debugging such a problem for new layouts. But it can and has happened.

How do we mitigate it? (methods for avoiding it while designing a layout and also methods for fixing a board already suffering from it?)
Try to isolate high frequency signals or signals that have the potential to reach high frequencies. Surround the signal with a healthy ground plane or track. Do not cross these signals over others unless it's isolated with a ground route (more possible with multi layered PCBs). If trying to remedy a PCB with a crosstalk problem, cutting the track at the source of the signal and route with a shielded cable is the easiest method to salvage the board.

-KM

[EATyourGuitar]

One of the reasons it doesn't matter is if a guitar pedal is all transistors under 800Hfe with average current consumption under 20mA it doesn't matter as much. As AC current through the power distribution increases, so does the chance of cross talk. Some cross talk is induction but some cross talk is from power modulation. The power distribution system is a resistor network because the resistance of copper is greater than zero. You can draw inductors and caps shorting everywhere to get an idea of how all this works for the induction part. For power supply modulation you can think about the resistor network of 0.0001 Ohm resistors. As you draw more current through a resistor the voltage drop also increases so you have a changing voltage where components connect to a power bus.

[FiveseveN]

I've always taken RG's caveat as better safe than sorry, in the sense that it's easier to screw up a layout if you just dump a ground plane without being aware of how the current flows.
So the answer is it very much depends on the circuit and layout. In some instances the difference between "plane" and "trace" becomes fuzzy:

[Rob Strand]

Ground planes help prevent signal noise/interference from outside getting into the circuit signals.    For digital and high frequencies it helps stop interference getting out.     Planes also help signals from one part of a circuit coupling into other parts.

Generally the only negative side effect for a ground plane is the increased capacitance.   You would need to have a very good reason to say increased capacitance is a big enough problem to not gain the benefits of the previous paragraph.   It would apply to a very small part of the circuit anyway.

The goodness of ground planes can be also be misused.   If you have circuit switching 50A near some sensitive circuits  you don't want one big ground plane since you don't want the noisy grounds from the 50A circuits going through the grounds of the sensitive circuits.    You would have separate ground planes for each part of the circuit then connect the ground planes in a manner which prevents the noisy circuit affecting the sensitive circuits.

[antonis]

Big ground planes save etching solution..!! 

[GGBB]

Ground planes help prevent signal noise/interference from outside getting into the circuit signals.    For digital and high frequencies it helps stop interference getting out.     Planes also help signals from one part of a circuit coupling into other parts.

If one ground plane helps, does two help even more? Say - the first plane on the bottom side, plus a second plane on the top side connected to the bottom ground plane only at one point (e.g. the ground wire connection).

Another issue I'm trying to understand is the best way to isolate grounds between sections of a pedal - such as the LFO and clock sections of an analog chorus or delay from the audio section. Would separate planes in opposite layers connected only at the common ground point work better (or worse) than separate paths or planes in the same layer?

Not concerned with digital at all.

[antonis]

Would separate planes in opposite layers connected only at the common ground point work better (or worse) than separate paths or planes in the same layer?

I think you deal with capacitor plates geometrical dimensions, Gord..
(in the mean of the farther away from common ground point the more capacitative behavior of the ground plane..)

[EATyourGuitar]

You can sandwich clock lines in between two ground planes on a 4 layer boarf. You can run clocks from charge pump supplies. Charge pumps come in every size. If you need less than 1mA, there is a charge pump for that. There are regulators in SOT-23. Everything can be simulated in LTspice if you have some idea about what information you need. If you want to know the ripple attenuation of a 7809 that is on the datasheet. I did this once. I think it is -40dB. Regulators do not eliminate ripple they attenuate ripple. It helps if you have a number for clock ripple that is acceptable to you. Work backwards from the engineering requirements. Then find real solutions you can simulate or build and test.

[Rob Strand]

I'm mostly assuming double sided boards here.   Multilayer boards allow sandwiching tricks like EATyouguitar mentioned.

An overriding comment regarding this stuff is more about being pragmatic than following a recipe.    Recipes often work but being pragmatic, by identifying problem areas and putting in defenses, does a better job with less.    That's a big help on a double sided board because our have to get your tracks though and that leaves limited area for ground planes.

Also, it's not a small topic so I'm not going to do a good job in a post.  There's many tips and tricks pages for PCB layouts on the web.   Use the ideas to solve/avoid specific issues.   However be careful about what problem is being solved.  It could be reducing EMI or keeping ground inductance low, things that might not be so applicable to audio.

If one ground plane helps, does two help even more? Say - the first plane on the bottom side, plus a second plane on the top side connected to the bottom ground plane only at one point (e.g. the ground wire connection).

It can definitely help and is unlikely to be detrimental.  A good deal of audio uses the ground plane as a shield - a shield to stop bad stuff getting into the audio, either from outside or from other parts of the circuit.  The more metal shielding you throw around something the better the shielding.  You want the shield to enclose the sensitive circuit.   There is a good enough point beyond which over doing it only adds minor improvements.  If in order to get the ground plane in you have move your tracks around such that it causes other problems then you might reconsider where to draw the line.

Another issue I'm trying to understand is the best way to isolate grounds between sections of a pedal - such as the LFO and clock sections of an analog chorus or delay from the audio section. Would separate planes in opposite layers connected only at the common ground point work better (or worse) than separate paths or planes in the same layer?

These parts of the circuit do have the some of the issues you see with digital.      There's two issues here. 

The first is shielding - here you are stopping bad stuff getting out.  Ground planes will help prevent the high frequency signals from getting into the audio, which can cause whistles, ticks and noise.    The shielding ideas for stuff getting out is identical for that getting in as mentioned above.

The second issue is how the grounds connect together.   Things like star grounds and avoiding passing noisy grounds through the grounds of sensitive circuits.  You can think about the way the grounds to different parts of the circuit as being single thin tracks.  The fact the ground is a plane is secondary.    Where the lines become blurred is when you rely on the large size of a ground plane to reduce noise on the grounds when the real problem is the noisy grounds are passing through the same areas of the ground plane as the ground for the  sensitive circuits.   This can sometimes work but it's hiding a problem rather than fixing the root cause.

A good example is the ticks from an LFO.   If you wire the power and ground for the LFO back to the input supply without passing through any audio you have the best chances of avoiding LFO ticks.   You could probably use thin power and ground tracks and it will still work because the solution is addressing the real problem.   Adding filtering on power rails will also help reduce the ticks  but that's different line of defense.

The most difficult thing out of all this to know what problem you are trying solve or avoid in the first place.

[GGBB]

Thanks Rob - quite helpful.

I am, in fact, looking for a recipe - at least a starter recipe. The problems I'm trying to avoid are general - same ones as everyone I think - noise and tone loss. I understand that we need to be pragmatic, but we also need to have a solid starting point. Everyone starts with something. The trouble with tips and other info on the net is that it's sometimes inconsistent and usually missing explanation. "Use ground planes" vs. "better for audio that you don't" (RG). The why and how are rarely present - just the what. Without the why and how it's difficult to be pragmatic. Most of what I've found on the net is sort of obvious - basically "use ground planes" but no mention of how other than "it depends on what you are doing." It's like there's a secret society of people who know about this stuff and they are all in collusion to not let the rest of us know.

Your post helps with the why and how.

Funny thing is, I looked at images/artwork of a whole bunch of PCBs from various popular pedal PCB suppliers, and most seem to be following a pretty simplistic (dumb?) approach - ground planes on both sides connected to components on both sides - no signs of being careful about where your currents flow. That seems "wrong", but I can't find anyone saying specifically that. Just not a lot of good helpful info out there beyond the obvious.

Maybe for dirt pedals none of this really matters very much.

[Rob Strand]

I am, in fact, looking for a recipe - at least a starter recipe. The problems I'm trying to avoid are general - same ones as everyone I think - noise and tone loss.

The simplest recipe is what you called the "simplistic (dumb?) approach".   It definitely works more times than not.  Particularly where you want shielding, or, when you aren't mixing sensitive and noisy circuits.    There are some overriding caveats for example you would want to avoid the LFO supply currents from passing through the audio grounds.  You might also consider putting a large cap across the supply of the LFO and locate the cap near the LFO circuit so the pulse currents are confined around the LFO area of the circuit.

I understand that we need to be pragmatic, but we also need to have a solid starting point. Everyone starts with something. The trouble with tips and other info on the net is that it's sometimes inconsistent and usually missing explanation. "Use ground planes" vs. "better for audio that you don't" (RG). The why and how are rarely present - just the what. Without the why and how it's difficult to be pragmatic. Most of what I've found on the net is sort of obvious - basically "use ground planes" but no mention of how other than "it depends on what you are doing." It's like there's a secret society of people who know about this stuff and they are all in collusion to not let the rest of us know.

With difficult topics it's always difficult to generalize.  You are really dealing with specific and minute details.   There's many angles to consider and the simple recipes are about as far as you can take it without adding the finer specifics.   Also you have to see the circuit as a 3D object all connected together by non-ideal wires and coupled by capacitors which aren't parts but are the capacitors formed between wires, tracks, parts.   EMC and RF engineering have the same issues, people call it black magic but it's not really.  It's where physics and circuits meet.   It requires a different way of looking at things.  (and yes, it makes it hard to be pragmatic.)

Be interesting to know why the reasoning behind RG's comments.   He could have been stung in the past on some project.

One thing about pedals is the circuits are generally put in a nice metal enclosure which helps enormously to shield from outside interference sources.   You only have to deal with noise from the circuit itself.   That's why we have got away with single sided PCBs in pedals for years.   Barely a ground plane or large region of copper in site.    Maybe that's an underlying reason for RG's comment.    The Boss pedals do make some effort to use large copper areas where they can.

IMHO Behringer have done quite a good job with their PCB considering it's a plastic enclosure.   IIRC, the base is metal and grounded but the plastic enclosure means you need to get the shielding from the PCB.     Behringer use a lot of ground planes.   They pretty much pack as much grounded copper in as they can.    SMD parts also help because the small circuit area picks up less external interference and it leaves more space on the PCB for ground planes.  A lot of modern consumer products are the same, plastic enclosure and large ground planes.

This is an example of a Behringer board.
https://farm7.staticflickr.com/6217/6300243177_9d7326470c_z.jpg

If you want recipe where to focus attention for shielding aspects of ground planes.  (In some of these cases the ground plane will help prevent noise on the grounds as well.)
- The circuits towards the input side of high gain circuits.   
  If you have a multi-stage amplifier, a 1uV interference at the first stage gets amplified by all the stages and appears
   as a large level at the output.  The same 1uV interference signal at the last stage will remain small at the output.
- Noisy circuits, especially where the signals have sharp edges.   The couple through the high-pass filters formed
  by the stray capacitances between the wires.   Ground plane will help prevent the noise getting out.
- High impedance circuits, or points in the circuit where high impedances meet.    In this case stray capacitive coupling
  can do more damage because the high-pass filter form by the capacitance is lower due to the high resistance.
- Inputs tend to be more sensitive to noise because they are high impedance.   By when connected to a low impedance
  output they are not no longer exposed since the low impedance output prevent noise getting in.
- The guitar input is always high impedance and at the first stage so it's going to be exposed to noise and interference.
   That also connects to the footswitch.
-  Any long wires, for example input jacks at the top of the enclosure feeding down to a footswitch in the lower part of the
   enclosure.
- Keeping these sensitive lines close to ground planes and away from noise parts of the circuit is always a good plan.

Funny thing is, I looked at images/artwork of a whole bunch of PCBs from various popular pedal PCB suppliers, and most seem to be following a pretty simplistic (dumb?) approach - ground planes on both sides connected to components on both sides - no signs of being careful about where your currents flow. That seems "wrong", but I can't find anyone saying specifically that. Just not a lot of good helpful info out there beyond the obvious.

It's not a bad plan and will work most of the time.    If there's no overly aggressive or sensitive parts in the circuit it's unlikely problems will arise and the ground plane will provide good generals shielding.    For a high gain pedal for example the biggest enemy would be noise getting in.  The ground plane helps fend that off.   It's unlikely there are strong ground currents so no problems chucking everything on same ground.   Where you might come unstuck is where the ground plane forms a loop but given each stage is kept to a small area the loops are likely to be kept small.    For a phaser most all parts of the circuit deal with similar level signals.  It's only the LFO you have to worry about.

[EATyourGuitar]

Notice most pedals have the LED connected to power but the audio circuit has an RC low pass filter on power. Something like 47R 10uF. Already there are two power busses. This is different from the idea of separate grounds but it is also similar. The LED doesn't need a filter because it doesn't matter if there is ripple on the LED. Some circuits are sensitive to noise and some circuits create noise. From the place where the analog ground and digital ground connect all the way to the power entry there is common impedance coupling on the shared power copper. The two ways to address it is with super low impedance path or with no coupling. This would be 2oz copper or 4oz copper on power supplies. Star grounding directly at the power entry is how you avoid common impedance coupling. If you don't have 2oz copper and you are not building power supplies then the next option is polygon lands or super wide copper traces. A ground pour on both sides gives you a low impedance path on the ground only. It doesn't address modulation on V+. That pioneer PCB that was posted in this thread is an excellent example of good polygon land for everything. Study it. Also notice that components are placed at 90 degree angles on amplifier boards to prevent cross talk through induction.

[Rob Strand]

Here's some articles that make a few good points,

http://www.ikonavs.com/OptimisedForAudio.pdf

http://home.iitb.ac.in/~pradeepsarin/students/tether/generalectronicsfundaes/adv/TexasInst_Opamp_PCB_Layout.pdf

[R.G.]

Grounding is mysterious because good grounding practice forces us to think about where, exactly, the ground currents flow in the ground conductors, not so much where the voltage is. Ground currents flow in the lowest impedance path from their source to their load. At DC, only resistance matters, as inductive impedance is zero and capacitive impedance is near-infinite. As frequency rises, trace inductance particularly dominates until some frequency where capacitive impedance lets the current leak off into free space.
Audio mostly counts as "DC" for these purposes. Fast rising/falling edges of switched signals have harmonics into broadcast RF regions, and the edges "see" the inductive impedance.
You get low inductive impedance by making broad, flat traces. A plane is the ultimate extension of this. Wide traces can help with both low DC impedance and low inductance. Again, this might not matter to audio.
What really gets you with audio is not being careful about where the DC resistances lead your currents. Especially ground currents.
Luckily, with audio you can force currents to flow only where you want it to by running specific traces for each current. If you let the ground currents from two or more different circuit sections, their currents mix in the traces, and the "ground" voltage in each section is different. Since most of our circuits have little or no ground noise rejection, this "ground" voltage difference can get amplified by the high gains used in some pedals.
A ground plane is usually good, as it allows ground currents to flow wherever they want, and that is usually from source to load of the current. It doesn't mean that there aren't ground current induced voltages there, only that they're generally smaller because the resistance and inductance are low. The down side of Ground Planes Everywhere!! is that this approach can induce extra capacitance and hence treble loading on high impedance traces, like the inputs to FET opamps, JFET and MOSFET gates; and the side effect that it can make soldering difficult and repairs/modifications very difficult.
I've typed in descriptions of the four or five different kinds of "ground" here before. My fingers are tired. A search should find it.
Planes are ... a tool. Like any tool, they have good applications, like a hammer for nails. They have works-OK-nothing-special uses, like a hammer as a paperweight or door stop. They have poor uses, like a claw hammer's claw used as a screwdriver.

[amptramp]

Ground planes generally have some provisions like etched arcs around the holes so it doesn't take excessive heat to solder to the plane.  Some people like an open mesh ground plane so it isn't as likely to warp if you try to tin- or solder-plate the whole board.

One thing to think about is using circuitry that doesn't create as much noise.  A bipolar 555 can be swapped out in favour of a CMOS 555 or better yet, an LFO can be redesigned as a phase-shift oscillator rather than something timer based.  Even if you need a dual pot to get the control range you want, it may be worth it and a phase-shift oscillator does not inject much noise into a power or ground plane.

[R.G.]

One thing to think about is using circuitry that doesn't create as much noise.

Excellent point. Stopping noise by not generating it is an excellent first step.

One trick that just came to my mind is using power domains - power and ground sections that are separated by filtering and specific-purpose power traces. Tube amps universally do one version of this, by introducing dropping resistors and filter caps for each one or two tubes. This attenuates any power noise between the tube sections. Tubes, in common with common emitter or common source amplifiers have zero power supply noise rejection. Tube amps missed the boat by not in general using star grounding, which is the other half of power domains.

[GGBB]

Here's some articles that make a few good points,

http://www.ikonavs.com/OptimisedForAudio.pdf

http://home.iitb.ac.in/~pradeepsarin/students/tether/generalectronicsfundaes/adv/TexasInst_Opamp_PCB_Layout.pdf

Quite a few good practical ideas there - thanks again.

I've typed in descriptions of the four or five different kinds of "ground" here before. My fingers are tired. A search should find it.

I've probably read them all - thanks. It's not the knowing of that stuff that I struggle with, it's how to use those tools.

The down side of Ground Planes Everywhere!! is that this approach can induce extra capacitance and hence treble loading on high impedance traces, like the inputs to FET opamps, JFET and MOSFET gates.

Exactly. So where do I go from there? Is it all or none? If I have a high impedance input (one circuit I'm laying out at the moment is 5M), can I run the ground plane around those sections or do I have to leave the ground plane out entirely?

One thing to think about is using circuitry that doesn't create as much noise.

Excellent point. Stopping noise by not generating it is an excellent first step.

Which unfortunately is a luxury not available a lowly builder of clones such as me.

--

All the tips - thanks everyone - and reading has me leaning toward a ground plane on one side only laid away from high impedance inputs. Ground planes on both side sounds like just more (double?) capacitance on traces with very little noise benefit if any.

What I'm not sure about is whether the ground plane should be on the same side as the circuit traces or the opposite side. Is having the ground plane flow between traces (same side) more helpful than having a continuous ground plane (opposite side)? I'm torn.

The context here is purely analog simple DIY clone type pedals - mostly dirt boxes.

[Rob Strand]

All the tips - thanks everyone - and reading has me leaning toward a ground plane on one side only laid away from high impedance inputs. Ground planes on both side sounds like just more (double?) capacitance on traces with very little noise benefit if any.

IMHO shielding around high-impedance circuits is more important than capacitance (there's always specific cases where you might pull the other way).
 
You should play with some PCB calculators to see how large the capacitance really is.

https://technick.net/tools/impedance-calculator/microstrip/

You might see 40pF/m to 100pF/m so a 50mm long track is <  5pF.      That's the same order is the input capacitance of a transistor buffer.    For opamps it's always wise to incorporate a cap from the output to the -input to ensure stability in the presence of opamp input capacitance and pcb capacitance.

[jonny.reckless]

This is such a complex subject and could fill a whole book.  There's a lot of great practical advice here already. Here's some of my thoughts gained over doing mixed signal audio PCBs for 20+ years. You can get decent performance out of a 2 layer PCB if you are careful.

You need to think about where currents flow, and power supply domains. The higher the frequency, the more the mirror currents want to flow closer to the outgoing current. Keep loops small, and the higher in frequency you go, the smaller the loops need to be. Decouple anything with fast edges or high frequencies with short, fat traces. Minimize the slew rate of fast edges whenever practical, you want to keep dv/dt and di/dt as low as possible within the constraints of the speed / bandwidth of the circuit design. For example a small capacitor from output to inverting input of an op amp relaxation oscillator will slow down the slew rate and reduce the "ticking" problem at source.

Don't share copper with signals that can destructively interfere with one another. For example, in an audio power amp with traditional bridge rectifier and smoothing caps, there are large current pulses at 120Hz when the diodes in the bridge conduct to charge up the reservoir capacitors. Keep the traces for this completely separate from anything else. The copper is not a superconductor and these pulses will appear superimposed on your clean audio signal otherwise.

Star point grounding works well from DC up to about 1MHz or so. It's great for all analog designs in the audio frequency spectrum.

In a mixed signal circuit with any type of clock or flip flop, e.g. a relaxation oscillator, keep the power supply and ground current pulses away from sensitive audio signals. You can get coupling from ground impedance, or for fast edges, capacitive coupling to high impedance audio nodes. Keep both the power supply and ground return current pulses local, and away from sensitive signals. Decouple power and ground pins with high quality ceramic caps with short leads and short fat traces to minimize inductance. The old 100nF decoupling cap folklore is obsolete. With modern MLCC caps I generally use 1uF or even 10uF decoupling caps on anything which might switch currents quickly. It's all about the plate size and lead inductance. For fast digital stuff and microcontrollers you want to use several decoupling caps of different sizes and values to lower the Q, but that's a separate discussion.

Every ground path has a resistance, inductance and capacitance. The relative importance of these depends on signal frequency and impedance, and you need to apply judgement and experience to determine what is best. Planes work well for homogeneous circuits with high frequencies. Mixed signal is a bit more involved. You often have to cut planes or have multiple planes to get the best analog performance. This really starts to matter with high fidelity codecs. A 24 bit codec with 110dB dynamic range can be reduced to <60dB dynamic range by poor grounding and decoupling practices.

A copper pour with lots of gaps, cutouts or breaks in it is NOT a ground plane, as the mirror currents will be forced to traverse circuitous routes, spewing electromagetic interference with abandon 

My approach for basic through hole pedals is to try and route everything on the bottom copper layer. Use the top layer for "links" i.e. short straight traces for when you need to jump over tracks. This leaves 99% of the top layer of copper available for ground. Once you've done the copper pour, take a good look and make sure there aren't any breaks, gaps, cuts or otherwise circuitous or high indutance paths that need to be addressed. You can then fill the remaining bottom layer with ground pour and couple it to the top layer with vias. This won't be a ground plane on the bottom layer, it's too fragmented for that, but it can provide a nice electrostatic shield. You might not want this near to guitar input signals, MOSFET gates or otherwise high impedance nodes where the distributed capacitance will kill the treble. And keep specific grounds on their own traces. For example, power supply grounds and speaker return grounds in an amplifier should have their own, fat traces connected directly back to the star point.. In my PCB designs I have a star point component that lets me name different grounds, and connect them specifically at one point, thus enforcing the correct grounding topology using the tool.

Hope this helps you a bit