[sdiy] Various GND planes in PCB layout..

[harrybissell]

Hej Magnus :^P

uhh yeah, what he said

Most of us s-diy folks aren't using planes, I assume that this is
a professional question.

BTW has anyone seen the 1Hz to 160MHz VFC that Jim Williams just
got in EDN ???   (url is for .pdf file)

http://email.ednmag.com/cgi-bin2/DM/y/enMU0Eil3C0Dar0CZYp0EK

He has an area that is specified to be 'air insulated' and NOT over a ground
plane.

H^) harry


Magnus Danielson wrote:

> 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
> > > >
> >