Going 4 layers...

[JAY X]

Hi!

I'm considering going to use 4 layers pcb for my next audio layouts. I know there is a thread explaining the pros and cons and how to layout things... Ok so far.

In my case I used to use two layers and used wire jumpers for all connections that crossed other traces on the top layer, in order not to trace anything on the bottom layer, and maintain the bottom gnd plane uncut. It worked well, and also used stitching for copper areas. All this worked well.

Now, the easiest way for me to go to 4 layers is to replace all top layer jumpers, with traces on the bottom layer, maintain SIG/PWR on top layer as I always did on my 2 layers boards, and, as the second and third layers are just copper with no traces, and are stitched with all the 4 layers, I think it could work, because the bottom layer traces have their return path in the third layer, and the top layer signal/power will have their return path in the second layer.

I know it is more complex than this, but I think all this makes sense, and the only way to prove it works is to order some boards...
Just wanted to share my thoughts because I feel I'm entering the unknown zone....

Jay x

 

[Matador]

I would consider following a "hierarchal ground" (e.g. ground follows signal) strategy for your ground routing, rather than relying on pours that span the entire plane. This opens up the "bottom" layer for routing jumpers and/or other traces. It also reduces the chances of ground pollution from noisy nodes, and forces you to think about how ground currents are returning back to their source.

 

[JohnRoberts]

4 layers make it a lot easier to layout but can be difficult to troubleshoot and/or modify if important traces are hidden on an inner layer.

JR

 

[Newmarket]

Pros and cons to all strategies but I would recommend just going standard. Use one inner layers for OV and the other for Voltage rails ( number of as required). Signal traces top and bottom. I have approved / designed several boards this way including audio. No issues with the layer stack.

 

[JAY X]

Hi!

Ok!, thanks! , very good advices!. I also have seen, read, that whenever you route a track from top to bottom layer, always place a via to gnd near the trace so to comply with Gnd follows signal...So, maybe I need to place a bit more vias to GND in the right place...

Attached is an excerpt of my layout..

Note:
Blue is Top layer
Dark Brown (not shown) is the second layer.
Light Brown is the third Mid layer
Green is Bottom layer.

 

[ruffrecords]

I think there is some confusion surrounding ground follows signal. The advice is normally meant for PCBs without a ground plane, the idea being to place a ground trace under a signal trace in order to minimise loops area which can cause or be susceptible to interference. With a complete plane of ground. every trace already has ground copper underneath it. Ground return currents will actually preferentially flow in the copper beneath signal trace so you automatically have ground follows signal. No need for extra vias.

Cheers

Ian

 

[Newmarket]

I think there is some confusion surrounding ground follows signal. The advice is normally meant for PCBs without a ground plane, the idea being to place a ground trace under a signal trace in order to minimise loops area which can cause or be susceptible to interference. With a complete plane of ground. every trace already has ground copper underneath it. Ground return currents will actually preferentially flow in the copper beneath signal trace so you automatically have ground follows signal. No need for extra vias.

Cheers

Ian

Yes. There is the "Picket Fence" concept where you also have "0V fill" on the signal later but that is often not of real help ime. To put in context - 4 layer stack offers easier and more efficient layout. And a very large advantage in terms of rf immunity.
Think of all the good large consoles built on 2 layer and (all else being equal) 4 layer is the icing on the cake. And yes we have much more "rf pollution" now so it becomes more significant.
And inner Power/ 0V planes give you additional decoupling capacitance.

 

[abbey road d enfer]

I think there is some confusion surrounding ground follows signal. The advice is normally meant for PCBs without a ground plane, the idea being to place a ground trace under a signal trace in order to minimise loops area which can cause or be susceptible to interference. With a complete plane of ground. every trace already has ground copper underneath it. Ground return currents will actually preferentially flow in the copper beneath signal trace so you automatically have ground follows signal. No need for extra vias.

I don't fully agree.
With a groundplane covering the whole area of PCB, you end up with uncontrolled connections between dirty and clean grounds.
It has to be taken in consideration for PCB that contain preamps, power amps and PSU.
Even for a simple PSU, one must make sure that the AC connections, rectifiers and reservoir caps are isolated from the DC outputs.

 

[Newmarket]

I don't fully agree.
With a groundplane covering the whole area of PCB, you end up with uncontrolled connections between dirty and clean grounds.
It has to be taken in consideration for PCB that contain preamps, power amps and PSU.
Even for a simple PSU, one must make sure that the AC connections, rectifiers and reservoir caps are isolated from the DC outputs.

Well yes - but I think it's implicit that small signal / large signals / psu circuits need to minimise their common impedance.
For similar circuits a single 0V plane offers a very good solution given the low impedance.
There are subtleties. Henry Ott (rip) and Keith Armstrong (Cherryclough Consultants) are very good on this in terms of articles. Even if I think Armstrong is a bit off point when he uses audio applications as an example wrt Shield / Pin 1 / Signal 0V.

 

[ruffrecords]

I don't fully agree.
With a groundplane covering the whole area of PCB, you end up with uncontrolled connections between dirty and clean grounds.
It has to be taken in consideration for PCB that contain preamps, power amps and PSU.
Even for a simple PSU, one must make sure that the AC connections, rectifiers and reservoir caps are isolated from the DC outputs.

I would not disagree with the above but I would argue that those are separate 0Vs that need to be joined at some controlled point. Each one can be a separate ground plane.

If I was being pedantic I would point out that I never said the plane covered the entire PCB, but that it was complete; but that is semantics. Grounding is a complex subject.

My reply was mainly in response to the ground follows signal comment and the suggestion of adding extra vias.

Cheers

Ian

 

[ccaudle]

whenever you route a track from top to bottom layer, always place a via to gnd near the trace

That is a consideration when you have signal bandwidths in the hundreds of MHz or GHz and multiple ground planes in a high layer count board. Not much of a performance consideration in a 4 layer audio layout.

 

[Matador]

With a groundplane covering the whole area of PCB, you end up with uncontrolled connections between dirty and clean grounds.

I recall doing the calculation for the frequency when the Gaussian distribution of return current follows the signal wire within one 10mil trace width on each side (e.g. the path of least inductance), and if memory serves it was around 200 kHz (and above).

Well yes - but I think it's implicit that small signal / large signals / psu circuits need to minimise their common impedance.

True, but even small(ish) traces on a PCB satisfy this requirement for all but a handful of edge cases.

 

[ruffrecords]

I recall doing the calculation for the frequency when the Gaussian distribution of return current follows the signal wire within one 10mil trace width on each side (e.g. the path of least inductance), and if memory serves it was around 200 kHz (and above).

We discussed this some time ago and I seem to remember posting a video by an EMI consultant who demonstrated that it is clearly detectable at 10KHz in a ground plane. I will see if I can find it.

Edit: Here is is:



The relevant part begins around 4 mins 30 secs in.

Cheers

Ian

 

[abbey road d enfer]

I recall doing the calculation for the frequency when the Gaussian distribution of return current follows the signal wire within one 10mil trace width on each side (e.g. the path of least inductance), and if memory serves it was around 200 kHz (and above).

My concern is not EMI/RFI. It's just about minimizing pollution of sensitive nodes by dirty currents.
Low frequency stuff. Ohm's law. Kirchoff.

 

[Wavelength]

Gang you can think of everything in loops. Also not one way is correct for everything. Like when I do amps I do segmented star grounding. So everything for that node is connected then star grounded back to the CT of the HIGH voltage. When I do digital or analog work and it's all pretty low current I flood a plane and leave it for everything to attach. In the past they said that was terrible and to isolate the analog and digital. A couple of friends who worked on CD/DVD products for Philips found that it wasn't a good idea to do that. That one gnd plane for all was much better. They also found that putting the negative side of the cap really close to the ground terminal and running the longer trace to the VCC was better than the opposite.
If you have a high current loop mixed with low current, then you really need to watch your loops. I usually take the high current and loop that back to ground and leave that off the ground plane. Leaving the plane to the low level signals.
Another thing back when we used tape it was always traces vertical were red and horizontal were blue. With the use of multiple layers and good thought in placement that is no longer required. I did 3 boards last week, one 4 layer and two 2 layer. The 4 layer was an SPDIF->DAC module that I could have done in 3 but didn't make sense. The DPLL required a bit of routing and it was mixed SMD and through hole so all the SMD was on the bottom layer. Anyway the other two flood the bottom layer each one had a short 1 trace on the bottom but I also flooded the top and then sticked it together with vias. All good that way and the ground is really firm on both.
One thing I never do is use a layer for power. Your just creating a cap and not a good cap between that and the ground plane. I also flood signal areas and then tie them through stiching with vias to the ground plane. That acts like a shield for analog signals and beefs up the ground in those areas.

 

[abbey road d enfer]

Like when I do amps I do segmented star grounding. So everything for that node is connected then star grounded back to the CT of the HIGH voltage.

I agree with most of your post, except for segmented star ground.
You end up with long trace between stages, which gives an opportunity to develop differential voltage between "grounds", particularly if ripple is important. The only way to minimize them is to use balanced or ground-sensing connections.

 

[MidnightArrakis]

With my having once been a "Senior PCB Designer" involved with the successful design of countless multi-layer PCBs with rather complex "Power & Ground" layers and routing, particularly with a well-known U.S. space agency that I cannot name because another member of this forum despises me of doing so and who now has me blocked and ignored, I could possibly offer and/or provide some useful insight into how the OP could configure and route his 4-layer stackup, but.....based upon the fact that my postings are usually reported as being -- inappropriate -- even when making a joke, all that I can offer now on this topic is.....NO COMMENT!!!

SORRY!!!.....Jay X!!!

By the way.....from the time when "double-sided" PCBs were manually hand-taped using adhesive-backed colored Mylar tape, the "standard" routing layer colors were:

Layer-1 -- TOP -- RED

Layer-2 -- BOTTOM -- BLUE

Then, when computer monitors switched from being either "Black & White" or "Green & Greenish-White", to being basically "color monitors" with at least 16-colors, the multi-layer colors were "agreed upon" as generally being:

Layer-1 -- TOP ROUTES -- RED

Layer-2 -- GROUND -- GREEN

Layer-3 -- POWER -- MAGENTA

Layer-4 -- BOTTOM ROUTES -- BLUE

/

 

[abbey road d enfer]

Thank you for setting the record straight, but, was the first paragraph necessary? Or even interesting?

 

[Cqwet Dbdfte]

4 layers make it a lot easier to layout but can be difficult to troubleshoot and/or modify if important traces are hidden on an inner layer.

JR

Never terminate a trace to a thru hole part on an inner layer. (Note to self)

 

[Cqwet Dbdfte]

I don't fully agree.
With a ground plane covering the whole area of PCB, you end up with uncontrolled connections between dirty and clean grounds.
It has to be taken in consideration for PCB that contain preamps, power amps and PSU.
Even for a simple PSU, one must make sure that the AC connections, rectifiers and reservoir caps are isolated from the DC outputs.

You can still segment poured ground areas with a "exclude" line or similar technique. Even a zero width trace (not connected) will force a ground path, it will generate some DRC error to be ignored.
Via fence or "via stitching" along signal traces is standard practice to increase isolation.
Put a few ground vias close to each decoupling capacitor, and part ground.
I make my mounting holes grounded, but if concerns are ground loops, solder-jumpers can be placed on these later solder blobbed as needed.
High impedance and high voltage areas get restrictions on ground pours, but otherwise I pour ground on all layers.
This may have been labor intense in the "tape era".
Generally SMDs go on the "top" and thru hole on the bottom, then install the board SMD down, with minimal traces on thru hole side.
I pour ground on all layers, heavily stich everything including along edges (edge plating is an option).
Thermal reliefs are great for easy manufacturing and hand soldering with wimpy soldering irons, but with modern 70W irons and easy-change "tips", and 63/37 solder I ditched thermal reliefs many years ago.
https://encrypted-tbn0.gstatic.com/..._FfQ2W3h1bEHV-yxoCloTLwg9txHuDgVKsc1L0I0lSpc4