Ground planes and analog ground on densely route boards...

[mb300sd]

It's almost always suggested by datasheets to have separate analog grounds and ground planes, but I'm just not seeing how to do it on a really dense board. For example, the current one I'm working on:



It tends to be a struggle just avoiding excessive numbers of vias for the last 10 signals or so, and traces are already spaced at the minimums for the manufacturer.

[doctormord]

Is this a 2 or or 6 layer board? You may use a commong ground plane for everything but you have to make sure that the digital return pathes arent crossing any analog return path. This is somewhat frequency dependant. Without a bit more information about the chips n stuff, i can't help any more.

[Sebastian]

I would recommend that you don't split it, unless you know what you are doing, because otherwise you can easily make things worse than with a solid gnd plane.
As doctormord said, you have to take the current return paths into consideration, and if you don't do so, and just split the gnd plane you could get EMI problems.

[mb300sd]

2 layer boards. I'm a hobbyist designing for personal use only, so I'm not really concerned about EMI unless its so bad it actually starts messing with stuff in my house. Board shown is a STM32F4 with DP83848 ethernet PHY, but I'm more looking for general suggestions on how to do it (if it's even possible) without going to a 4 layer board at twice the price.

[doctormord]

Beside the GND-planes, I'd consider to realign the headers on the left, with SWD on top, then SPI, then USART. If this is not going to work, switch USART for SWD, if possible. Also the right bottom USB can be rerouted when having a GND-Fill. You'll need to get your D+- tidier. The actual routing is far from optimal with room for optimization. For your GND, i will get you some information later, i have to look for my bookmarks.

A good practice is to start with is the sensitive analog signals first, then the clocks and high speed buses.
Regards, doc

Edit:

Here they are:

Start here:
http://www.hottconsultants.com/tips.html

http://www.hottconsultants.com/techtips/split-gnd-plane.html
http://www.hottconsultants.com/pdf_files/june2001pcd_mixedsignal.pdf
http://www.hottconsultants.com/pdf_files/ground.pdf

http://www.learnemc.com/tutorials/guidelines/Worst_Guidelines.html

http://www.e2v.com/content/uploads/2014/02/0999A.pdf
http://www.icd.com.au/articles/Split_Planes_AN2010_6.pdf
http://www.elmac.co.uk/pdfs/Lord_of_the_board.pdf

More complicated:
http://muehlhaus.com/support/ads-application-notes/momentum-port-global-ground-or-differential
https://awrcorp.com/download/faq/english/docs/Simulation/axiem.html

[mb300sd]

Actually the USB, USART, and SPI were an afterthought tacked on for future expansion and/or GPIO when I saw there was extra room on the board, so I'm glad those were the ones you found issues with

The headers on the bottom are for the main application, connecting a second stacking board with an audio CODEC, where I'm trying to keep noise down as much as possible. It'll be a bit less dense so I should be able to place a ground pour shielding it from the high speed signals below and keep all the digital IO on the 1 corner where the headers are. The Top left and center headers are placed where they are for mechanical support, and are for wire connections (using extra long header pins).

Thanks for the links.

[Bassman59]

It's almost always suggested by datasheets to have separate analog grounds and ground planes.

Those datasheets, generally like the parts they describe, are obsolete.

[tggzzz]

It's almost always suggested by datasheets to have separate analog grounds and ground planes.

Those datasheets, generally like the parts they describe, are obsolete.

In fairness, split ground planes can be useful, provided you understand the small number of reasons for splitting and the consequences thereof. Often, of course, the purported reasons are fallacious and the consequences not understood.

Usually non-split is best.

[daqq]

Offtopic: Couldn't help but notice: you have vias in SMD pads - a bad practice, avoid if possible.

[tggzzz]

Offtopic: Couldn't help but notice: you have vias in SMD pads - a bad practice, avoid if possible.

Sometimes recommended, e.g. when decoupling GHz signals you really don't want any unnecessary track length @ 1nH/mm

[T3sl4co1l]

Offtopic: Couldn't help but notice: you have vias in SMD pads - a bad practice, avoid if possible.

Sometimes recommended, e.g. when decoupling GHz signals you really don't want any unnecessary track length @ 1nH/mm

Or internal lands (QFN, LGA) where there's no room for fanout and where thermal or electrical performance demands it.

Like many things, it's a practice which is generally recommended against, but has important exceptions.  The duty of the engineer is to make an informed decision when making those exceptions.

Tim

[mb300sd]

Offtopic: Couldn't help but notice: you have vias in SMD pads - a bad practice, avoid if possible.

Sometimes recommended, e.g. when decoupling GHz signals you really don't want any unnecessary track length @ 1nH/mm

Or internal lands (QFN, LGA) where there's no room for fanout and where thermal or electrical performance demands it.

Like many things, it's a practice which is generally recommended against, but has important exceptions.  The duty of the engineer is to make an informed decision when making those exceptions.

Tim

Is there a reason for that other than it absorbing the solder paste during reflow? I never used to do it but it makes routing easier and I haven't heard of any other issues as long as the boards are hand soldered.

[T3sl4co1l]

That's basically what it comes down to, manufacturing yield.  If you're doing it one-at-a-time and reworking until it checks out, you can do whatever you like.

Vias 8 mil or under are generally considered small enough not to be likely to wick solder.  Micro, filled and plugged vias are small enough, or have no opening whatsoever, and can be used in-pad at will.  They may add cost (as your supplier?).

Tim

[Rerouter]

All signals follow both the path of least impedance and path of least inductance, the faster the transition speed, the more it preferences the path of least impedance.

This is why you tend to see analog and digital  segments grouped by function, to keep currents from one segment overlapping another, you do not have to go as far as is-landing the analog segment on its own plane in most cases, just try and keep the overlap to a minimum.

Now breaks / islands in a ground plane are OK, as long as no signals cross the break and there is no large currents flowing along either side of the break, not following these 2 points will turn the break into an antenna, the larger the detour a signal has to take from its path of least impedance, the more noise it will emit, which may then be coupled back into your analog segment that you separated in hopes of preventing.

If you treat all signals as loops, it is easier to visualize what may become a problem, so a digital signal from your ADC feeds a bit of current out to your micro, this current will continue back through the micro, down its ground pin, and back through the ground plane the ADC's ground pin, completing its loop somewhere inside the ADC.

[nctnico]

In addition to that you can get the same effect by splitting power supplies using a ferrite bead or even a filter. A ferrite bead (of filter) will keep HF currents confined to an area of a PCB. You can still have capacitive coupling between a digital an anlog section.

[DerekG]

Is there a reason for that other than it absorbing the solder paste during reflow?

Board production costs will be more as 8mil drills break more often & more care is required to ensure such small holes plate through satisfactorily.

If you ordered 10,000 circuits containing quite a few 8mil via holes within pads, it is very likely you would have some failures. Your board supplier would often pick these failures up with their bare board conductivity testing. As the expected yield will be lower, quoted board costs would normally be higher.