[sdiy] Various GND planes in PCB layout..

[Magnus Danielson]

From: harrybissell <harrybissell at prodigy.net>
Subject: Re: [sdiy] Various GND planes in PCB layout..
Date: Thu, 01 Sep 2005 12:39:15 -0400
Message-ID: <43172EB1.35E3C008 at prodigy.net>

> One often overlooked point of ground and power planes... is that source and
> return currents will take the same path (the magnetic fields will cause them to
> run parallel on opposite sides of the board.

Well almost. The higher frequency, the more of the current will go in the
straigest path possible since that is the path of least inductance. Cut an
opening in one of the planes, and you have just created an inductance in series
with the powerline, cut both is better but not good. For very low-freq designs
such as pure audio, pure resistance is usually of most concern, but a star-
ground is certainly a good way to improve things.

For a digital signal (with sharp edge compared to the analogue) expect least
interference if the signal has an unbroken ground-plane below it from source
to destination. The return-current will take that path. However, one must
recall that it is actually both power planes which is coupled, so de-coupling
of the source and destination chips allows either of them act as low-inductance
path. Do not cut the power-plane and try to avoid having other signals between
the power-plane and the signal. Jumping between layers with vias is another
thing to be avoided. For lower frequency stuff, you want things on a quite
plane. which you can create by taking a normal power-plane and create a cut-out
area around it except for a small narrow bridge. Over that bridge will the
signals in and out go, but not over the cut in the planes. Low-freq current
will not pass through the quite ground due to the cut-out, but will pass
throught the rest of the plane. High-frequency stuff will follow their signals
anyway.

> They are NOT evenly distributed across the plane.  The "islands" mentioned
> will cause some of that current to be diverted on one side or another... making
> the current flow in a larger loop. That will cause noise to be radiated.
> 
> A flip side of this is that by cutting the planes into sections, you can force
> the
> current to take ANOTHER path.  You can force the analog currents to go one
> direction, and the digital another direction.
> 
> One tip for split planes... do not overlap them.  Keep analog power and ground
> opposite each other, and don't extend either one over a digital plane area.

Indeed.

There are numerous books that provide good reference and reading.

Cheers,
Magnus

> H^) harry
> 
> Jay Schwichtenberg wrote:
> 
> > Bert,
> >
> > If done right yes you can use the same analog ground. Typically where you
> > have problems is where there isn't enough copper to get enough current to
> > where it needs to go. So if you have 'strong/good' path and a 'weak/poor'
> > path more current will go though the 'strong/good' path and this may
> > unbalance the ground or power in portions of the circuitry. If you have a
> > major amount of copper going around the board you will probably be fine.
> > Here's another thing to watch out for. When you have something like your
> > digital section in the middle of the analog section you got to make sure
> > that the path around the digital island has enough copper to support the
> > current. An example would be you have point A upstream in a river and point
> > B downstream. Then put an island in the river. Depending on the size and
> > placement of the island the water is going to flow around it differently.
> > What you want to do is place the island so that you get even, smooth flow of
> > water all around it.
> >
> > As the other person mentioned I would be weary of putting the inductor in.
> > You have an active component in the ground that can change properties on you
> > and thus change the ground plane. The only place I can really remember
> > seeing inductors on both sides of power is on AC lines for noise
> > suppression.
> >
> > Hard core PCB layout is some pretty deep dark magic. If you haven't ever
> > seen any RF stuff you should see what the RF guys do. There the PCB is
> > actually part of the circuit. Pretty much for what we do here just sticking
> > to basics as far as PCB and circuit design will carry us a long way.
> >
> > Jay S.
> >
> > > -----Original Message-----
> > > From: owner-synth-diy at dropmix.xs4all.nl
> > > [mailto:owner-synth-diy at dropmix.xs4all.nl]On Behalf Of Bert
> > > Schiettecatte
> > > Sent: Thursday, September 01, 2005 12:58 AM
> > > To: jays at aracnet.com; synth-diy at dropmix.xs4all.nl
> > > Subject: RE: [sdiy] Various GND planes in PCB layout..
> > >
> > >
> > > Hi Jay,
> > >
> > > > I don't know if I would put an inductor on the ground. What
> > > > I've done before when working with audio converters is the following:
> > > >
> > > > 1) Connect the digital and analog ground at one and only one
> > > > point. Make sure the trace is big enough to handle the
> > > > current. Put this near where the power comes into the board
> > > > and before it is used by the digital section.
> > > >
> > > > 2) The system that I was working with shared +5V for both the
> > > > analog and digital components on the board. The primary was
> > > > analog +5V. To get the digital +5V we would use either a
> > > > ferrite or a small value resistor (10 to 20 ohms) between the
> > > > analog and digital +5V. Then we would bypass the +5 at the
> > > > resistor or ferrite with a larger value cap (4.7uf to 22uf)
> > > > and each digital chip had a smaller 0.1uf bypass cap. Also
> > > > make sure the resistor/ferrite can handle the current.
> > > >
> > > > Might want to get some of the application notes and/or audio
> > > > converter data sheets from Analog Devices, Crystal or AKM and
> > > > check out their PCB layout notes.
> > >
> > > Thanks for the tips. So if there are several different audio
> > > Circuits distributed around the PCB and around the digital
> > > Section (which is in the middle of the board), do they all have
> > > To share the same analog ground copper pour on the top? I also
> > > have a Ground plane since this is a 4 layer board, but I'm not
> > > sure I  Should split that up into an analog ground section and
> > > a digital Ground.
> > >
> > > Since the analog sections are all around the digital section
> > > In a circle, if I all give them the same analog ground copper
> > > Pour on the top layer, they will form 75% of a full circle
> > > Around the digital section. People told me making loops with
> > > Pcb traces is a bad idea so that's why the idea came up to give
> > > Each analog section its own ground copper pour on the top layer.
> > >
> > > Thanks!
> > > Bert
> > >
>