Multi layer PCB (more than 2)

[JohnRoberts]

Wow! Gareth, thank you so much for an in depth answer. This will benefit many people. All contributions will, I'm sure.

Regarding the CAD program, I use Eagle. I have the old version before they moved to the subscription based model. I have considered buying into that but after playing with the newer demo version, decided for what I do, I don't need the new features. There have been many threads here about CAD programs so we need not go there.

The debugging problem is the biggest downside, as many pointed out, and probably why I will stick with 2 layer for now as most of the projects I do now go very slowly, and rarely turn into a final product that will be duplicated.

This should probably be in its own thread, but I will bring it up anyhow...

boji! great video, that guy needs to chill on the Red Bull, Lol...

Pick and place service, my current PCB company only offers a template for solder paste. Can anyone explain quickly how it works when you get SMD components soldered to the final board? Do you submit a BOM and the company has standard parts already? Do you send an order of parts to the PCB company? How exactly does that work?

Is your version older than eagle-4.03? I still use the old eagle seat purchased for me back when I was still consulting (for money).

I don't recall the names of the specific  CAM routines but Eagle can generate X,Y parts placement location files as well as component placement angles (0,90,180).

The last time I ran a 250 pc board run my contract manufacturer was able to work from the BOM and CAM files generated by eagle. 

JR

 

[boji]

It's always been a point of pride for me to route a 2-layer board with no 'extra' vias (because again, evey PTH lead is a via), and I'll spend a bit of extra time moving stuff around to get all extra vias removed....done is always better than perfect.

Noobish anecdote:  I was so obsessed with avoiding via's on a relay card last year I lost the big picture; by optimising for traces instead of RJ placement, some wires leave the back only to bend around and go to other devices in the front... :
Not a show stopper since it's all inside the frame, but still...ugly mistake.  Had vias been used it would have saved meters of wire in total, and connections would make more sense to someone trying to service it.

Anyway, super awesome post. Thank you BB for the OP and everyone for shared wisdoms!
Edit: you guys kinda made my saturday afternoon...  <3

 

[john12ax7]

This, in overview, is what works for me as a 4-layer stack and has been proven to be highly successful:
Layer 1 (component side): inter-component signal traces & any other short point-to-point traces (decoupling caps to ICs).
Layer 2: Groundplane.... all of it.... no breaks.
Layer 3: Signals & power, mainly signals.  Flood open spaces with power or ground.
Layer 4: Signals & power. Ground flood of open spaces.

Thanks Gareth for such a detailed and informative post.

Your stackup is how I've typically done RF and mixed signal with layer 2 being the ground plane. With typical  pre-preg thickness you end up with the ground only 10 mil or so away from the audio signal which increases capacitance.  It would seem this is a non-issue then for typical audio?

I suppose the main question is,,for a 4 layer analog audio only board, is there an optimal layer to use for ground plane.?

 

[bluebird]

Is your version older than eagle-4.03? I still use the old eagle seat purchased for me back when I was still consulting (for money).

I think its 5 something so most likely has that functionality.

I was You Tubing around for "pick and place" (thanks boji ;D) and found this KID building his own pick and place machine. Absolutely amazing. He has many vids, building all kinds of things with a 3D printer. Just extraordinary skills.

https://www.youtube.com/watch?v=dAFleHaPjEY&list=PLIeJXmcg1baLBz3x0nCDqkYpKs2IWGHk4&index=1

 

[Gareth Connor]

Thanks Gareth for such a detailed and informative post.

Your stackup is how I've typically done RF and mixed signal with layer 2 being the ground plane. With typical  pre-preg thickness you end up with the ground only 10 mil or so away from the audio signal which increases capacitance.  It would seem this is a non-issue then for typical audio?

I suppose the main question is,,for a 4 layer analog audio only board, is there an optimal layer to use for ground plane.?

Cheers John, thank you.

My choice of groundplane layer for all-analog pro-audio design is layer 2.

The short answer is that the increased capacitance due to proximity is not a problem in almost all scenarios where signal paths are low-impedance. The situation changes somewhat when we are dealing with circuits such as equalizers, which by their nature can have many capacitors in the design and where controls create varying impedances, often quite high, resulting in interconnects that are sensitive and/or prone to the infuence of unintended picofarads. The controls may be several inches of trace-length (or wire-length) away from their associated circuitry. Here, capacitive inches of trace (or wire) can throw down the "banana skins" to cause design slip-ups. Maybe it's a case of luck or intuitive designing, but this has seldom been a real-world problem in the designs that I have been involved in. An exception to this was when stray capacitance resulted in having to change the value of a low-nanofarad cap to the next value down (IIRC it was something like 2n7 dropped down to 2n2) to compensate for an unusually long trace run that was surrounded by copper screening and pour. The important points being that the reason behind the wrong frequency could be analyzed, the problem defined and that there was a solution that was acceptable, repeatable, that did not compromise product performance..... with the bonus that no boards were scrapped. A good outcome for a one-off custom job.

 

[JohnRoberts]

Thanks Gareth for such a detailed and informative post.

Your stackup is how I've typically done RF and mixed signal with layer 2 being the ground plane. With typical  pre-preg thickness you end up with the ground only 10 mil or so away from the audio signal which increases capacitance.  It would seem this is a non-issue then for typical audio?

I suppose the main question is,,for a 4 layer analog audio only board, is there an optimal layer to use for ground plane.?

I'm no Gareth but my general advice for any layout is to visualize the current flows and imagine the copper traces and pours having higher resistance than they do,  so you can visualize and manage IxR voltage drops.

JR

 

[abbey road d enfer]

As I wrote earlier I do only 2-layer.
I route the "ground" and make sure it runs along signal. If for some reason, it has to go across I make sure the copper pour does not connect a ground string with another. In practice, it means creating several polygons that meet only at a chosen point (usually the main 0V reference point).
If this separation is not respected, the remote-ground sensing benefits of running signals and ground hierarchically will not happen.

 

[JohnRoberts]

The OP should do whatever floats his boat... Since I am cheap 2 layer is in the sweet spot for low cost low volume manufacturing.

If you tried to order a single sided PC board these days you would get one run across a 2 sided process with copper etched off one side... and most likely the same price as 2 sided.

A couple years back I ordered a no-sided board to act as a rigid battery hold down clamp to keep the batteries in place during shipping drops. I suspect that no-sided board had copper etched off both side...  The no-sided PCB was likely cheaper than me having bare FR4 cut to size with holes drilled in it by some job shop (and a lot easier).

JR

 

[Matador]

At least as of today, a typical quote for a 5"x5", 2-layer, green FR4, 62mil, 1oz copper board in quantities of 100 is about $1.50.  The exact same board, in 4 layer, from the same supplier, is about $3.  So despite being double, when you factor in the cost of a typical DIY BOM for an audio project, it's almost nothing percentage wise.

 

[JohnRoberts]

At least as of today, a typical quote for a 5"x5", 2-layer, green FR4, 62mil, 1oz copper board in quantities of 100 is about $1.50.  The exact same board, in 4 layer, from the same supplier, is about $3.  So despite being double, when you factor in the cost of a typical DIY BOM for an audio project, it's almost nothing percentage wise.

I wonder if the cost differential is only 100% for low volume orders. 

The cheap proto boards typically get panelized together with as many other projects as will fit on a common panel (12"x18"... guess).

It would seem that the material differential should make even less of a difference for small volume proto runs, but I would speculate that the 2 sided process is more automated (no human touches) than with more layers.  Humans are more expensive, even in China. 

JR