[sdiy] PCB layout rules

[Harry Bissell Jr]

Sounds pretty good...

I'd mention that the non-inverting input
of an opamp is just as sensitive as the
inverting.  Maybe if you are in the habit
of grounding that pin, it might seems like
its "OK" but it isn't.  Your suggestions about
Agnd should have covered that but "it ain't
necessarily so..."

Decoupling caps...

One per IC power pin per voltage... so the tpyical
opamp gets two.

Check out layouts of my evil-twin-separated-at-birth
(Jim Patchell) who does an excellent layout job.
We have the same style ~so~ close you might not be
able to tell our layouts apart...

The "Muffy" schematics over at (the late) Larry
Hendry's site show similar techniques

H^) harry





--- Joe Grisso <jgrisso at det3.net> wrote:

> 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
> >
>