[sdiy] Eagle analogue & digital groundplanes

Sarah Thompson plodger at gmail.com
Fri Nov 27 02:19:32 CET 2015


Yes, that was a spendy board, I think about $1k each as I remember, but
they had to make the thing small (500+ components on a 2.5" square board is
challenging). The reason for the 0.003" traces was partly dealing with mil
spec vias which are bigger than normal, so thinning the traces made it
easier to get everything in. Impedance wise the board house did a really
good job -- the TDR tests came out pretty much dead on. The board has 8
DC-DC converters on it, so there's a bit of power and switching going on,
as well as some RAM, a big-ish FPGA, some analog stuff, some comms, etc,
and it was really too small to easily separate all of that. I didn't do too
badly, but adding the extra power and ground planes made everything a lot
more straightforward. Frequencies on there are up to about 100MHz digital
with a mixture of LVTTL and LVDS, maybe 50MHz analog though there's also
some DC-100KHz stuff. Something for everyone, I suppose... :)

Sarah

On Thu, Nov 26, 2015 at 5:33 AM, Roman Sowa <modular at go2.pl> wrote:

> 3 mils traces? Not every PCB fab can make this. And at that trace width
> the edges will be relatively ragged quite a bit, so not so much controlled
> impedance.
>
> I want a job at NASA too :)
>
> Roman
>
> W dniu 2015-11-26 o 12:51, Sarah Thompson pisze:
>
> 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
>>>
>> _______________________________________________
>> 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/20151126/841b942a/attachment.html>


More information about the Synth-diy mailing list