[sdiy] Eagle analogue & digital groundplanes

Sarah Thompson plodger at gmail.com
Fri Nov 27 02:12:38 CET 2015


Not my design! It was due to someone who won't do it like that a second
time!

A lot of real designs don't have an easy demarcation between analog and
digital, so the Goddard training was basically in favor of unspaghettifying
(my word, not theirs) the circuit so that the return paths don't cross, but
they basically made the argument that if you were tying the planes
together, you are still better off with a single plane. They backed it up
with experimental data.

Sarah

On Thu, 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.
>>>>
>>>
>>>
>>> _______________________________________________
>>> Synth-diy mailing list
>>> Synth-diy at synth-diy.org
>>> http://synth-diy.org/mailman/listinfo/synth-diy
>>>
>>
>


-- 
[s]
-------------- next part --------------
An HTML attachment was scrubbed...
URL: <http://synth-diy.org/pipermail/synth-diy/attachments/20151126/a2d9eefe/attachment.html>


More information about the Synth-diy mailing list