[sdiy] PCB layout rules

[Joe Grisso]

Matthias,

     I had written a quick set of rules I used back when I worked at
DOD Electronics in '97. Here's the pertinent part of the message:

--begin snippet--

Most of our designs are mixed signal, so they are very tricky to layout
so we don't get digital crosstalk, scanning noise from the switch/LED
muxes, etc. Only our low-end FX pedals are strictly analog, but they
still have things like bucket brigade devices on them that can make
routing a nightmare.
Here's some routing guidelines I tend to follow and apply to my own
home synth designs, as well as most of the boards we have here.

- Ana Power and Ground: These are the most critical traces globally, due
to
the required low-Z for good power supply performance.
We route these traces away from high-speed clocks or
chokes that can cause magnetic induction in the trace.
I use a 30 mil trace at minimum, with a 50 mil trace
preferred. In certain spots where I need to squeeze a
track through a very tight spot, I can go down to 20
mils on the track for less than 1/8". Also, in
situations where I need to shield a quiet area from
a noisy area (I.E: from a BBD clock), I use generous
ground plane area on both layers around the circuitry
to be protected, with a no-copper "moat" in between
the noisy circuitry and the sensitive circuitry. One
large point here is that if you have two planes to
isolate noise, you should have a *SINGLE POINT*
connecting each plane together. This is to minimize
reflections and noise from the noisy plane entering
the "quiet" plane. The "moat" should be at least 100
mils wide.

- Signal Traces: Signal traces are the second most important. Make sure
you lay out your board to minimize long-haul traces
between circuit blocks. Also, when using op-amps, keep
the trace connecting components to the inverting input
of the op-amp *AS SHORT AS POSSIBLE* This is very
important, because noise can be easily induced into
the inverting input. Also, keep these traces as wide
as possible. We use a minimum track width of 12 mils,
and a preferred track width from 18 to 20 mils. Keep noisy
components and traces away from the input and output stages of the
audio signal path, at least 100 mils. This will prevent noise being
coupled/induced in the input and output of your signal.

- Balanced Signals: If you have a balanced signal path, there is a
simple
set of rules to follow to ensure proper transmission
of balanced signals on your PCB. If you use 12 mil
tracks to layout a balanced design, make sure the
distance between the high and low side is EXACTLY 12
mils. All other signals must be 24 mils apart.
Technically speaking, For track width W, the distance
between adjacent signals on a balanced pair must be
W apart, and the balanced pair must be spaced 2W or more from all
other signals, if possible.


- Control Traces: Follow all of the guidelines specified in "signal
traces" above, except that the minimum trace width can
be 10 mils in most cases.

- Mechanical Issues: Most board houses, if you opt to get a board
fabricated at a bureau, will allow you to design a
board with a minimum trace width of 8 mil, and minimum
pad/via size of 40 mils with a 20 mil hole diameter.
These are ABSOLUTE MINIMUM LIMITS. Wherever possible,
use thick traces, and be generous with pouring power
and ground planes. If you are doing only single-sided
boards, think about the mechanical problems. Make your
pads 10 to 30 mils larger, because it will give the
copper on the board more surface area to hold on to
the PCB substrate, and will lower the thermal impact
on the underlying glue that holds the copper to the
board. Also, it provides a better mechanical bond for
front panel components like Pots, Switches, LEDs, etc.
When you place mounting holes in/near power and ground
planes, be sure you place a "no copper" area around
the mounting hole to prevent shorting the chassis to
the board. If this is not possible, be sure to use a
minimal "no copper" area, and then use a nylon washer
to isolate the chassis from the circuit board.

Hope this is a decent primer in analog layout techniques. If everyone is
interested enough, I'd like to continue this with a small addendum that
explores mixed signal design.

--end--

I should revamp that layout guide to include the new state of the art,
but those rules above apply for most homebrew designs.

To give a good contrast between capabilities back in '97 and now, most
bureaus back then could fab an 8mil (0.008") trace, and really picky
bureaus could get down to 6mil (0.006"). Today the state of the art
sits at 3-4mil (0.003"), and minimum drilled holes can go down to 8mil
now. However, if you need smaller holes you can use laser drilled ones
that will get down to 4mil. Multilayer boards have also become much
less expensive, so dedicated power and ground planes are much more
economical to do. We also have RoHS to deal with, which involves
higher temperature materials that the board is fabricated with.

I hope this gets you off on the right foot!

Happy Holidays,

Joe Grisso
Detachment 3 Engineering


On 12/21/06, Matthias.Herrmann at jeppesen.com
<Matthias.Herrmann at jeppesen.com> wrote:
> hi list,
>
> there was a recent talk about PCB layout software. some recommended to
> avoid the use of autorouter for audio circuits.
>
> so now i wonder what are the drawbacks or pitfalls?
> what are the main rules for layout design? (i.e. how to organize gnd,
> power, audio, cv tracks)
> when and where are bypass caps needed? allways as near to the ICs as
> possible?
>
> many thanks in advance
>
> cheers,
> matthias
>