Four-Layer PCB Stackup

From circuitbending to homebrew stompboxes & synths, keep the DIY spirit alive!

Moderators: Kent, Joe., luketeaford, lisa

Post Reply
User avatar
Chris Willocks
Common Wiggler
Posts: 101
Joined: Mon Dec 09, 2019 1:09 pm
Location: England
Contact:

Four-Layer PCB Stackup

Post by Chris Willocks » Thu Jul 23, 2020 5:46 pm

Just wondering if anyone could offer any advice regarding a generic, four-layer PCB stackup suitable for low-speed, audio, analogue modules. I’m currently using two layers, however I can purchase four-layer PCBs for only slightly more, so I’m looking to improve the performance of my modules by upgrading their PCBs to four layers. One issue I’ve run into with two-layer PCBs is large cuts in the ground planes as they are shared with signals on both layers, which isn’t ideal.

Anyway, from doing a lot of reading on the web, I have the following stackup in my mind:

Top layer: signal traces + power traces (VCC)
2nd layer: common reference plane (GND)
3rd layer: common reference plane (GND)
Bottom layer: signal traces + power traces (VEE)

This is essentially figure 7 in the following article: https://www.allaboutcircuits.com/techni ... ayer-board.

My idea was to route VCC (+12V) traces on the top layer with signal traces and the same on the bottom layer for VEE (-12V). A common four-layer stackup I’ve seen seems to have a power plane on the 3rd layer instead of the common reference plane, however I’m not sure how this would work with multiple power rails?

It states in the above article that power pours or a gridded power configuration could be used on the top and bottom layers, however I presume that standard power traces would suffice for low-speed, audio applications i.e. synth modules?

Another concern with the above stackup is that through-hole components would produce cuts in the common reference (GND) planes, however I presume that this would be negligible and still be an improvement over the two-layer stackup of signals and common reference pours on both sides?

Anyway, just wanted to know if the above stackup seems suitable and any further advice would be much appreciated.

Thanks,
Chris

User avatar
cackland
Super Deluxe Wiggler
Posts: 2207
Joined: Thu Dec 28, 2017 5:42 pm
Location: Los Angeles, California

Re: Four-Layer PCB Stackup

Post by cackland » Thu Jul 23, 2020 6:09 pm

I was going through this recently and from my understanding and research, I was lead to believe the following was a suitable 4 layer stack:

Top Layer: Signal traces + GND pour;
2nd Layer: PWR or GND (If Top Layer has more significant traces than Bottom Layer, place GND);
3rd Layer: PWR or GND (If Bottom Layer has more significant traces than Top Layer, place GND);
Bottom Layer: Signal traces + GND pour;

Would be good to get feedback from more experienced designers than myself.

JanneI
Wiggling with Experience
Posts: 382
Joined: Mon Oct 19, 2015 3:28 am

Re: Four-Layer PCB Stackup

Post by JanneI » Thu Jul 23, 2020 6:13 pm

My non-EE opinion is that these things largely vary depending on the actual PCB size. If you can manage to get solid ground plane with 2-layers, I'm not sure if there's a real advantage with 4-layers. If space is really limited, then 4-layer makes sense, especially with SMD components. As long as it's analog signals only kind of board, one has to really screw up things to get measurable differences. With digital one needs to be more careful.

I've simply used:
top: signal
1st inner: power rails
2st inner: GND plane
bottom: signal

I'd be interested to hear EE comments for these analog only SDIY PCB designs. If I'm completely off here, correct me.

User avatar
Chris Willocks
Common Wiggler
Posts: 101
Joined: Mon Dec 09, 2019 1:09 pm
Location: England
Contact:

Re: Four-Layer PCB Stackup

Post by Chris Willocks » Thu Jul 23, 2020 6:28 pm

Thanks for the replies both. Most of my modules (except simpler ones like mixers, mults etc.) have well populated PCBs component-wise, so the ground planes/pours on either layer of a two-layer PCB are usually too spliced up to be optimal or neat. Also, I have a good mix of TH and SMD designs, so I think four-layers would be sensible.

User avatar
emmaker
Veteran Wiggler
Posts: 706
Joined: Sat Mar 10, 2012 5:07 pm
Location: PDX

Re: Four-Layer PCB Stackup

Post by emmaker » Thu Jul 23, 2020 8:49 pm

Unless you're doing some dense, high frequency, sensitive (uV, mV range) or analog/digital hybrid circuit in my not so humble opinion (actually I'm a f'n ass) this is overkill for SDIY and don't think this will gain you anything. I think learning good, basic PCB skills and not trying to pack a PCB as densely as possible would be better. I haven't done more than a 2 layer board in 25 years and back then we'd do stuff as in fig. 1 and fig. 2 in the article. The author didn't say much about frequency that I saw. So the point of the new 'stack' is to help with noise and EMI which is typically higher frequency stuff if so is that going to benefit SDIY, I don't know.

Here goes my rant about some DIY PCB issues. Probably more than what you want to hear and indirectly answers some of your questions.

I think and I maybe wrong here that most people look at a PCB they have and go 'I can do that' and mimic what they see without really understanding what is going on. Good chances are they're looking at a board that was made to be machine assembled (not something that is made for DIY hand soldering) or they are coping techniques done by someone that doesn't know what they are doing. An example might be the small pads used for thru-hole parts. This is SDIY stuff not something soldered my a machine and probably not reworked. You might want to change a gain stage by changing resistors. A lot of DIYs can't solder well and have bad rework skills. Big pads don't lift as easy as small ones.

When ever I see a DIYer doing plane fills I figure they don't know what they're doing and are just mimicking what they have seen.
  • You've touched on this above. I'd like to see the analysis the designer did showing if the power routing can carry the current to the circuit properly or that the path isn't 20" long creating more resistance than needed. If you route these as traces you will know for sure what the current carrying is and the length of the trace.
  • Some people use a very small fill gap between the plane and traces, vias and pads. This can do the capacitor/inductor thing depending on frequency and current of the circuit. Another issue is if the plane solder mask gets damaged near a solder joint it's easy to get a solder bridge between the plane and solder joint. Remember this is SDIY and a lot of people are really bad solders.
  • Some people use ground planes for crosstalk issues. First do your traces right and that can avoid a lot of crosstalk issues. Second proper guard tracks are a better solution.
  • They don't use thermal pads and if they do the traces to them won't carry current since they are to small.
  • People don't get rid of the islands not connected to anything and just leave them on the board. In high frequency and in some high power circuits these can act as capacitors and inductors.
  • Using plane fill makes it hard to hack (remember this is SDIY, people like to tweak this stuff) the board. Basically with a plane fill you don't have any place to drill holes, add components and wire them in. You have to add components on top/bottom of the board where they can be mechanically unstable unless you glue/attach them to the board someway.
End of rant.

Other things to think about that are more pertinent.
  • With 4 layer boards think long and hard about what you're putting on the inner layers. Once the planes or traces are there they will probably be hard to impossible to modify if there are issues. You might be able to drill out pads, vias or traces and do rework on the top or bottom of the board but if you can't you're screwed.
  • Might think about having one layer being power ground and one analog signal ground. Probably not going to be an issue unless something uses a lot of current like LEDs, 555s, ... or is noisy like digital chips or uCs.
  • Depending on what you are doing you may end up with all sorts of power and grounds so you might not use plane fills and use traces the proper size for the current. I've worked on a project that had high current/digital/analog power and high current/digital/analog/signal ground. Just make sure that the traces are big enough to carry the current. Also if you have multiple power supplies and a single ground the ground has to carry all the current for all the supplies.
  • Always draw current through a bypass cap unless you absolutely can't. Do 'power -> cap -> load' and not 'power -> load -> cap'.
Someone with to much time on their hands.
Jay S.

User avatar
EATyourGUITAR
has no life
Posts: 5798
Joined: Tue Aug 31, 2010 12:24 am
Location: Providence, RI, USA

Re: Four-Layer PCB Stackup

Post by EATyourGUITAR » Thu Jul 23, 2020 9:38 pm

JanneI wrote:
Thu Jul 23, 2020 6:13 pm
My non-EE opinion is that these things largely vary depending on the actual PCB size. If you can manage to get solid ground plane with 2-layers, I'm not sure if there's a real advantage with 4-layers. If space is really limited, then 4-layer makes sense, especially with SMD components. As long as it's analog signals only kind of board, one has to really screw up things to get measurable differences. With digital one needs to be more careful.

I've simply used:
top: signal
1st inner: power rails
2st inner: GND plane
bottom: signal

I'd be interested to hear EE comments for these analog only SDIY PCB designs. If I'm completely off here, correct me.
starting on page 456 the bible of PCB manufacturing talks about stack up and ground planes. I tried to scan these 3 pages for you but my scanner broke just now. they say this is a bad idea. they say you want every routing layer next to a ground layer. your top signal layer is too far away from a ground plane. the idea here is that electricity flows in a circuit so you will always complete the circuit with ground. you can punch through a single layer of dialectric with a short via of a known size and impedance. in this way you can keep a low impedance path to ground always. you can put your bypass caps in ideal positions with low impedance grounding. most of these rules are for 10MHz signals but they are not bad rules to follow even if you don't need them. SD cards need equal length traces with controlled impedance.

I will tell you a hack though. to save money, you can do a stackup definition that puts all vias on to all layers. this keeps all the drill holes uniform across all layers. it eliminates an extra masking process at the fab. therefor saving a lot of extra work and money. you might not be able to use this on a fine pitch BGA. you said you are only doing analog though. a saw core oscillator needs to follow the guidelines of high frequency circuits. analog comparators, turing machines, these are analog but not really analog you feel me?

WWW.EATYOURGUITAR.COM <---- MY DIY STUFF

JanneI
Wiggling with Experience
Posts: 382
Joined: Mon Oct 19, 2015 3:28 am

Re: Four-Layer PCB Stackup

Post by JanneI » Fri Jul 24, 2020 3:07 am

EATyourGUITAR wrote:
Thu Jul 23, 2020 9:38 pm
I will tell you a hack though. to save money, you can do a stackup definition that puts all vias on to all layers. this keeps all the drill holes uniform across all layers. it eliminates an extra masking process at the fab. therefor saving a lot of extra work and money. you might not be able to use this on a fine pitch BGA. you said you are only doing analog though. a saw core oscillator needs to follow the guidelines of high frequency circuits. analog comparators, turing machines, these are analog but not really analog you feel me?
Thanks for the comments. You mean "hidden vias"? So far I've not used them, all vias are through all layers.

If you need a ground plane between all signal trace layers, 4-layers won't be enough, would it?

User avatar
EATyourGUITAR
has no life
Posts: 5798
Joined: Tue Aug 31, 2010 12:24 am
Location: Providence, RI, USA

Re: Four-Layer PCB Stackup

Post by EATyourGUITAR » Fri Jul 24, 2020 5:57 am

it only implies that every odd number signal layer be adjacent to at least one even number ground plane. conversely every even number signal layer must adjacent to at least one odd number ground plane. there is some truth to what EMMAKER said. for a guitar pedal or a distortion module, none of this shit matters. for a VCO, I think it does matter. I think maybe the one key point is that you are building a synth for yourself DIY, don't drop the ball because you are waiting for perfect. sometimes it is more important to finish a project and evaluate your mistakes rather than read this 1550 page book that costs $150. your time is a limited resource.

there is a difference between
tented vias
blind vias
buried vias

internet search will set you straight on the definitions. the idea is that a cheap PCB with 4 layer has no blind or buried vias. tented vias are possible for no additional charge. you don't ask for it, you simply put no holes in your conformal coating for micro vias when you process cam to make the gerber.

here is the code for eagle in design rules->layers->setup
(1*2*15*16)

this is the cheap 4 layer setup I was telling you about. there are no blind or buried vias.
WWW.EATYOURGUITAR.COM <---- MY DIY STUFF

jorg
Ultra Wiggler
Posts: 796
Joined: Fri Apr 03, 2015 9:38 am
Location: East Coast USA

Re: Four-Layer PCB Stackup

Post by jorg » Fri Jul 24, 2020 9:17 am

Avoid blind and buried vias, of course.

Signal - GND - Power - Signal would be a pretty standard stack. Put lots of decoupling between power and ground planes; the power plane should be made as clean as the ground plane because it will act as a ground plane.

User avatar
Chris Willocks
Common Wiggler
Posts: 101
Joined: Mon Dec 09, 2019 1:09 pm
Location: England
Contact:

Re: Four-Layer PCB Stackup

Post by Chris Willocks » Fri Jul 24, 2020 11:31 am

Thanks everyone for the replies and advice.
jorg wrote:
Fri Jul 24, 2020 9:17 am
Signal - GND - Power - Signal would be a pretty standard stack. Put lots of decoupling between power and ground planes; the power plane should be made as clean as the ground plane because it will act as a ground plane.
What would be the best way to integrate multiple rails i.e. +12V and -12V into the power layer? Would you use separate fills for each or traces?

User avatar
devinw1
Super Deluxe Wiggler
Posts: 1638
Joined: Tue Aug 07, 2018 11:20 am
Location: Portland, OR
Contact:

Re: Four-Layer PCB Stackup

Post by devinw1 » Fri Jul 24, 2020 11:57 am

I have a sweet presentation on PCB layout that one of our EEs got from a seminar. I'll grab it next time I'm on my work PC and see if i can upload it. It's pretty detailed.

jorg
Ultra Wiggler
Posts: 796
Joined: Fri Apr 03, 2015 9:38 am
Location: East Coast USA

Re: Four-Layer PCB Stackup

Post by jorg » Fri Jul 24, 2020 12:19 pm

Often the -12V is pretty sparse compared to +12V; it could be traces within the plane. But best to look at some tutorials to get the feel for it.

User avatar
cackland
Super Deluxe Wiggler
Posts: 2207
Joined: Thu Dec 28, 2017 5:42 pm
Location: Los Angeles, California

Re: Four-Layer PCB Stackup

Post by cackland » Fri Jul 24, 2020 10:34 pm

devinw1 wrote:
Fri Jul 24, 2020 11:57 am
I have a sweet presentation on PCB layout that one of our EEs got from a seminar. I'll grab it next time I'm on my work PC and see if i can upload it. It's pretty detailed.
Look forward to it :)

User avatar
cackland
Super Deluxe Wiggler
Posts: 2207
Joined: Thu Dec 28, 2017 5:42 pm
Location: Los Angeles, California

Re: Four-Layer PCB Stackup

Post by cackland » Sat Sep 19, 2020 5:48 pm

devinw1 wrote:
Fri Jul 24, 2020 11:57 am
I have a sweet presentation on PCB layout that one of our EEs got from a seminar. I'll grab it next time I'm on my work PC and see if i can upload it. It's pretty detailed.
Did you even manage to get a hold of this?

User avatar
ablearcher
Veteran Wiggler
Posts: 619
Joined: Thu Dec 26, 2013 8:00 pm
Location: Portland
Contact:

Re: Four-Layer PCB Stackup

Post by ablearcher » Mon Sep 21, 2020 10:26 am

The Henry Ott book ( and the Howard Johnson book ( are the standard references for layout.

The PCB stackup short page on the Ott site may be enough for audio though: http://www.hottconsultants.com/techtips ... -up-2.html

Keep in mind that audio layout is nearly trivial compared to RF. In EE world all higher speed traces -must- be run against an unbroken ground plane otherwise you run into EMI/EMC issues. The speed of audio signals doesn't really require that though.

Don't add random ground fills on a otherwise occupied layer, you might create an antenna and add noise to your design.

The best reason to use four layer pcbs in audio design is so that you can quickly route a pcb without spending days and days trying to route everything on one or two layers.

For four layer I've been doing:
top: components and critical signals
inner1: ground
inner2: horizontal signal and power traces
bottom: vertical signal and power traces

I do generally space the traces on inner2 enough that I can add a ground fill so that the copper is roughly symmetrical and won't create a warped board, not to act as a return path. You really need more layers to create a good return path for each layer, in which case it's good to remember that power layers can act as return paths. In eurorack modules though the current is low enough that it is okay to route power as traces (keeping them orthogonal on adjacent layers) instead of planes. You do want to route the power as a star or grid, not as a big snake from point to point though.

User avatar
devinw1
Super Deluxe Wiggler
Posts: 1638
Joined: Tue Aug 07, 2018 11:20 am
Location: Portland, OR
Contact:

Re: Four-Layer PCB Stackup

Post by devinw1 » Mon Sep 21, 2020 11:07 am

cackland wrote:
Sat Sep 19, 2020 5:48 pm
devinw1 wrote:
Fri Jul 24, 2020 11:57 am
I have a sweet presentation on PCB layout that one of our EEs got from a seminar. I'll grab it next time I'm on my work PC and see if i can upload it. It's pretty detailed.
Did you even manage to get a hold of this?
PM'd!

Post Reply

Return to “Music Tech DIY”