Prev: Build A Home Internet Business For Extra Income Stream
Next: LT Spice ideal diode
From: Colin Howarth on 4 Apr 2010 07:10
Hi,

I've just upgraded Eagle to the non-profit license, so I can now (in
theory :-) do 4-layer boards.


1. If I have a ground layer and I have one part as an analogue ground
plane and another as a digital ground plane (two adjacent rectangles)
how and where should they be connected?


2. Given that I have a ground plane, should I still do copper pouring in
the signal layers (and connect them to ground)?


3. This probably isn't relevant for my first project (guitar-computer
interface: differential signal, 192 kHz, 24 bit ADC with pre-amp and
USB/FW), but which is the cleaner solution for, say, a single signal
crossing: 2 vias with a trace on the bottom signal layer, or a zero ohm
SMD with the other signal passing under it?


4. One of the circuits I am copying/modifying has a 1uF / 63V
electrolytic decoupling capacitor (directly in the signal path) before
any amplification. Wouldn't a plastic (polyethyleneterephthalate) one be
better, from a noise point of view?


5. Is it OK/possible/desirable to place a via on an SMD pad (e.g. for
resistors & capacitors to ground)?


6. I suppose it's better not to route signals underneath opamps (from a
noise point of view)? What if the path then has to become a fair bit
longer? Is there a rule of thumb here?


Thanks for any answers!

colin
From: Bill Sloman on 4 Apr 2010 07:50
On Apr 4, 1:10 pm, Colin Howarth <co...(a)howarth.de> wrote:
> Hi,
>
> I've just upgraded Eagle to the non-profit license, so I can now (in
> theory :-) do 4-layer boards.
>
> 1. If I have a ground layer and I have one part as an analogue ground
> plane and another as a digital ground plane (two adjacent rectangles)
> how and where should they be connected?

The usual advice is to connect under the point where the signal goes
from analog to digital - the A/D converter, or the D/A converter that
provides the interface.

The thought that you should keep in mind is that every digital signal
track running over ground plane injects current into the ground plane
(via the track to ground capacitance) whenever the singal changes, and
you don't want this current to circulate througn the analog ground
plane (where it can produce voltage drops which can inject curent into
the analog signal traces.

> 2. Given that I have a ground plane, should I still do copper pouring in
> the signal layers (and connect them to ground)?

It's less urgently necessary, but it can still rovide extra screening.

> 3. This probably isn't relevant for my first project (guitar-computer
> interface: differential signal, 192 kHz, 24 bit ADC with pre-amp and
> USB/FW), but which is the cleaner solution for, say, a single signal
> crossing: 2 vias with a trace on the bottom signal layer, or a zero ohm
> SMD with the other signal passing under it?

Routing the signal so that there is always ground plane and /or power
plane between it and the second signal has to be better. At higher
frequencies, the vias introduce discontinuities in the "transmission
line" formed by the track running over ground plane, but this isn't
usually important at digital audio rates.

> 4. One of the circuits I am copying/modifying has a 1uF / 63V
> electrolytic decoupling capacitor (directly in the signal path) before
> any amplification. Wouldn't a plastic (polyethyleneterephthalate) one be
> better, from a noise point of view?

Perhaps. The film capacitor will have less leakage current, but it
will be bigger than the electrolytic, and consequently a better
antenna for electromagentic interference.

> 5. Is it OK/possible/desirable to place a via on an SMD pad (e.g. for
> resistors & capacitors to ground)?

It's not popular. The via can wick the solder away from the pad, and
prevent the component from forming a good solder bond at the pad.

> 6. I suppose it's better not to route signals underneath opamps (from a
> noise point of view)? What if the path then has to become a fair bit
> longer? Is there a rule of thumb here?

Not that I know of. A signal running over a buried ground plane isn't
all that effective as a radiator or an antenna, so routing stuff under
op-amps is less of a worry on a four layer board.

--
Bill Sloman, Nijmegen
From: John Larkin on 4 Apr 2010 10:54
On Sun, 04 Apr 2010 13:10:16 +0200, Colin Howarth <colin(a)howarth.de>
wrote:

>Hi,
>
>I've just upgraded Eagle to the non-profit license, so I can now (in
>theory :-) do 4-layer boards.
>
>
>1. If I have a ground layer and I have one part as an analogue ground
>plane and another as a digital ground plane (two adjacent rectangles)
>how and where should they be connected?

It' almost always better to have obe solid ground plane layer.
Splitting or slicing grounds generally causes trouble. Just manage the
analog part of your circuit carefully. It does halp to keep large
circulating currents away from low-level analog stuff. Really
low-level signals should be differential.

>
>
>2. Given that I have a ground plane, should I still do copper pouring in
>the signal layers (and connect them to ground)?

Not worth it.

>
>
>3. This probably isn't relevant for my first project (guitar-computer
>interface: differential signal, 192 kHz, 24 bit ADC with pre-amp and
>USB/FW), but which is the cleaner solution for, say, a single signal
>crossing: 2 vias with a trace on the bottom signal layer, or a zero ohm
>SMD with the other signal passing under it?
>
>
>4. One of the circuits I am copying/modifying has a 1uF / 63V
>electrolytic decoupling capacitor (directly in the signal path) before
>any amplification. Wouldn't a plastic (polyethyleneterephthalate) one be
>better, from a noise point of view?
>
>
>5. Is it OK/possible/desirable to place a via on an SMD pad (e.g. for
>resistors & capacitors to ground)?
>

A via in a pad can slurp off solder. Most people use a very short
trace between a pad and a via, just long enough to get some solder
mask on.

>
>6. I suppose it's better not to route signals underneath opamps (from a
>noise point of view)? What if the path then has to become a fair bit
>longer? Is there a rule of thumb here?

Depends on the signal. If it's unrelated to the opamp signal, like
another auidi thing or a digital thing, keep it away. If it's part of
the same signal, it's OK.

John

 | 
Pages: 1
Prev: Build A Home Internet Business For Extra Income Stream
Next: LT Spice ideal diode