[sdiy] Eagle analogue & digital groundplanes

[rsdio at audiobanshee.com]

Yes, thanks, Sarah. Lots of good information in your write-up, especially mentioning the online Goddard training courses.

I was going to bring up the same point as Richie. When I design four-layer boards with split ground planes, I never have signals cross planes. Even the mixed-signal chips that I use, like 1-to-16 analog multiplexers, keep the digital signals separate from the analog signals. I just place those chips so that the digital pins are over the digital plane and the analog pins are over the analog ground plane. Thus, no signal traces need to cross the gaps between ground planes. There have been a few exceptions that require strangely-shaped polygons for the ground planes, but after I get the shape right I still never need traces to cross gaps. I'm dealing with 4 MHz to 20 MHz digital signals and upwards of 60 kHz analog signals.

Brian


On Nov 26, 2015, at 9:45 AM, rburnett at richieburnett.co.uk wrote:
> Hi Sarah,
> 
> Thanks for the detailed reply.  I totally agree with everything you said about tracking from an EMC compliance point of view.
> 
> The only line I find strange is this one "Once you are into a few MHz, this is sufficient that if you try to make a signal span a gap across two planes it will pretty much get lost in the process".  Surely the whole idea of using separate ground-plane areas is that you DON'T try to make high-frequency signals cross a gap between two different planes?
> 
> All your low-frequency analogue things have return paths in the analogue ground plane, and all your multi-MHz HF things have return paths in the digital ground plane, and in an ideal world the two don't cross.  (The ADCs and DACs sit on the boundary of the two ground planes with digital traces leaving over the digital ground-plane and analogue traces leaving the other direction over the analogue ground-plane?)
> 
> Or are you saying that your design wasn't as simple as:  Analogue = Low-frequency,  Digital = High-frequency
> 
> I can imagine that things get a whole lot more complicated (and harder from an EMC compliance point of view) if you have to deal with very high-frequency analogue signals too!?
> 
> Best regards,
> 
> -Richie,
> 
> On 2015-11-26 11:51, Sarah Thompson wrote:
>> I got weened off my previous tendency to use split ground planes due
>> to the EMC training I got courtesy NASA Goddard (I works at NASA Ames
>> -- a lot of Goddard's courses are available online if you go digging
>> for them -- I'd recommend it, they made me a much better designer).
>> Basically, split ground planes do work at audio frequencies up to a
>> point, but they are terrible at higher frequencies. The short version
>> is all signals have a current return path across any adjacent ground
>> and/or power plane(s), which gets more localized as frequencies
>> increase. Once you are into a few MHz, this is sufficient that if you
>> try to make a signal span a gap across two planes it will pretty much
>> get lost in the process -- all of this energy ends up either radiated
>> as unintended EMI or splattered across your other signals or both. In
>> one case I saw a board, just about 4 inches square, where a 2.5V LVDS
>> clock at just 10MHz failed to get from one side of the board to the
>> other because it had to cross a couple of splits -- the effect is
>> actually very strong indeed. The right way to deal with this is to use
>> a single ground plane whilst being VERY careful with routing, being
>> cognizant of where the ground return paths are going and treating them
>> effectively as signals in their own right, with particular attention
>> to signals that cross each other on adjacent planes.
>> Where budget allows, adding extra ground planes is the secret special
>> sauce that makes problems go away. On one of my recent projects I did
>> a 12 layer stackup which went (top to bottom) signal, ground, signal,
>> ground, signal, ground, power, power, power, power, ground, signal.
>> All four signal layers were impedance controlled so that 0.003" traces
>> were 50 ohm to ground and 100 ohm between adjacent LVDS pairs. This
>> basically let me safely have multiple splits in the power planes,
>> since signals only ever ran adjacent to ground planes and no signals
>> ever crossed each other in adjacent planes. This was expensive, I'll
>> admit, but it allowed for a very small board with lots of high speed
>> digital, precision analog and 8 switching DC-DC converters with
>> absolutely no signal integrity issues even on the first spin. It was
>> all just done on EAGLE, no fancy SI tools were used.
>> Sarah
>> On Nov 25, 2015, at 11:29 AM, rsdio at audiobanshee.com wrote:
>>> I typically place an 0805 inductor link between analog and digital ground, near the analog supply regulator. In some cases, I've had to change the BoM from inductor to resistor or jumper. I think that placing the SMD pads there, in 0805 sizing, is a good step no matter how you connect the grounds.
>>> Professional layout engineers seem to do a lot of manual work, in which case I'd imagine that they just live with the DRC violations.
>>> I've read articles which claim that separate ground planes are not necessary - when placement and ground paths are properly controlled. However, I like to have the separate ground planes anyway, because it at least gives me a reminder of the ground paths that I've planned during placement. These articles talk about lots of stitching via links between layers for multiple ground planes, but that's only an option when you have the luxury of more than four layers, I'd say.
>>> Brian Willoughby
>>> Sound Consulting
>>> On Nov 25, 2015, at 8:18 AM, Richie Burnett <rburnett at richieburnett.co.uk> wrote:
>>>> Out of interest what are Eagle PCB CAD users doing to connect together their analogue and digital ground-planes?
>>>> A wire-link, 0805 zero-ohm link, or over-lapping the polygons for the analog and digital ground-planes and accepting a DRC violation at the point where they're connected?
>>>> Those are the best ideas I had, but wondered if there's a clever way to do it.
>