[sdiy] Aaron's first PCB layout

[Tom Corbitt]

IMHO you should never leave something like this up to the end user.
You really don't want to trust that someone will solder the correct
pins when you're talking about power and ground.The good news is that
on your design it's an easy fix, just drag the trace down below the
power connector and run it under the 2.2k resistor.

I think you did a great job on your first attempt (I wish my first
board looked as good) but if you were starting over, here is what I
would do

#1 design towards signal flow, for me this is the way I read, left to
right. but your mileage may vary.

#2 Place key parts first. For my work usually the constraints of the
enclosure drive this, but a close #2 is power. You did this, as all
the op amps are lined right up, but you failed to take advantage of
your placement. What you should have done is run the +/- 15 rails
straight down the center between the op amp pins, tagging out to the
pins. This frees up a lot of space right next to the device and allows
you to put your decoupling caps right at the top and bottom of the
device, which frees up the I/O pins for a straight shot (you should,
btw, have decoupling caps right next to each op amp something I'm not
seeing right now) This allows you to remove the large power pours, so
you don't have quite as much enviromental noise coupled into the op
amps. Always keep power as short and simple as possible and do it
first, you don't want to have to shim it in as an afterthought around
signal layers.

#3 Walk the schematic with respect to signal flow above, i.e. lay down
the parts for one op amp (but keep an eye out for the overall signal
flow). If it doesn't fit together well, rip it up and try a different
approach. The rats nest isn't always a friend when you are doing this;
often you'll miss a simple solution because the connections make you
think a part can't be moved but when you move it you find it will work
just as well somewhere else. I often find turning off common nets like
GND can help in some stages.

Single boards without jumpers are hard to do. I know it's easier to
etch at home, but the trade off in the amount of drilling you need to
do for a board like this would be huge (I etch at home, but I'm almost
completely surface mount in my designs.) I'd focus for now on doing a
good two layer board, treat the 2nd layer as a signal flow layer that
interconnects between stages (with the majority being a GND pour after
you've finished)

What has been said about planes/pours is true, but I think that as a
beginner, you're better off with a lot of ground pour, as often it
will help fix problems that you didn't see. The most important thing
is making sure that return currents have the simplest path home; you
don't want them having to run across/beside low level signal paths to
find the potential they seek. Star topology is great, but hard to
maintain on dense boards. On a board like this I'd recommend analog
islands, where you have an AGND that connects to the master via a
single zero ohm resistor (which you can be clever with and tie
together via a star) You want to be sure to rip up any dead copper
(copper pour that isn't connected to anything)

You can really get drag all the physics/electronics of coupling and
various cap and inductive effects between the traces and such, but
being in the analog realm you don't have to worry as much about such
things. Keep digital away from analog, sprinkle 0.1uF near any chip
and feed it good clean power.

Tom

P.S. When I started professional pcb design, a wise old engineer told
me about the various levels of PCB designers

The first is just getting everything down on the board. Then you shoot
for everything connected. Hopefully sometime during this stage you
make a board or two that works.
The second comes when you start to understand parts placement and
signal flow, hopefully you once again manage to make a few boards that
work
The third phase is when you learn enough to start to design for
manufacturing, lowering BOM part counts and making sure that the
boards are easy to make and such.
The last phase is when you have done enough boards that you know what
it will look like when you finish the schematic. When you get to this
point, it's about time to retire.



On Sat, Jun 7, 2008 at 7:46 PM, Veronica Merryfield
<veronica.merryfield at shaw.ca> wrote:
>>> 1) To avoid using jumpers, I run a signal line between the MOTM style
>>> ground pins. So this requires that the user be sure to apply ground to both
>>> pins. I'm not sure if that's good practice or not.
> I forgot to mention this other than the divided 0v. It is not a good idea to
> run one signal line right round a board like this because of noise/crosstalk
> pickup and because of any propagation time, but I assume this is probably
> not an issue. However, there is a path for that trace without going between
> the ground pins and without removing all the ground plane, although removing
> it that would make it easier.
>
> On 7-Jun-08, at 3:17 PM, mcb, inc. wrote:
>
>> On Sat, 7 Jun 2008, Aaron Lanterman wrote:
>>
>>
>> I don't know what the circuit is and I don't see the signal line but
>> I believe this would set off alarm bells among a lot of board
>> designers.  The signal return path for some number of signals
>> might all be through this 'signal' line.
>>
>> --
>> Monty Brandenberg
>
> _______________________________________________
> Synth-diy mailing list
> Synth-diy at dropmix.xs4all.nl
> http://dropmix.xs4all.nl/mailman/listinfo/synth-diy
>