Analog Layout Guidelines <was Re: PC boards, Requirements, and autorouters, oh my!>

[Joe Grisso]

bruce duncan wrote:
 
> Hi ,
> 
> I've experimented with protel's Advanced PCB autorouting functions and found
> the same conclusions.
> Especially if your track widths exceed 25mil and up which is more ideal for
> analog layouts.
> 
> I would be interested in any pointers as to what you consider when laying
> out a low-noise audio
> design in terms of  grounds and track widths etc.
> Do you have any basic rules of thumb or hints that you would be willing to
> share.
> 
> Always interested.
> Thanx
> Bruce
> 

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.

-- 
   __   ___   __
  /  \ / _ \ /  \  E l e c t r o n i c s
 / / // // // / /  -=-=-=-=-=-=-=-=-=-=-
/___/ \___//___/   C o r p o r a t i o n
==========================================
Joe Grisso - CAD Designer
jgrisso at dod.com