Notches in ground planes for multi-power multi-channel board

[namdeguerre@gmail.com]

All,

I am designing a multi-channel board and I have individual linear
regulators for each channel running off a common switcher.

Now, my concern is that due to the split power planes, which are like
thin fingers running through the board, I will cause potential
differences based on the current in different channels, especially,
because I have a common ground plane. Now, I was thinking my choices
are:

1) Split the ground plane as well, so I would have thin finger like
power and ground plane separated by narrow notch but connected at the
linear regulator end and at the input end. (All the channels are w.r.t
common ground plane.)

The trouble is, that I have common (to all channels) control lines
runnning across my planes (though separated by 2 layers) and even if I
isolate the grounds, some noise is bound to take the signal lines.

2) Keep split power planes, but add a narrow slice ground plane
between the power plane 'fingers' in between them on the same layer as
the power planes.

3) Keep 1, but put connections between ground planes at regular
intervals.

Anyone have thoughts on this. The voltages are +5 or less and it is
all analog..there are digital lines and a digital section, but they
come into the analog area through an isolator.

 

[Joerg]

All,

I am designing a multi-channel board and I have individual linear
regulators for each channel running off a common switcher.

Now, my concern is that due to the split power planes, which are like
thin fingers running through the board, I will cause potential
differences based on the current in different channels, especially,
because I have a common ground plane. Now, I was thinking my choices
are:

1) Split the ground plane as well, so I would have thin finger like
power and ground plane separated by narrow notch but connected at the
linear regulator end and at the input end. (All the channels are w.r.t
common ground plane.)

Splitting a ground plane is usually a recipe for disaster. I have yet to
see a case where that really worked and it's been decades now. In audio
designs it can work but only until a strong RF field shows up, upon
which all hell breaks loose.

OTOH if nobody split planes anymore I'd have less work so it does have
some upsides ;-)

The trouble is, that I have common (to all channels) control lines
runnning across my planes (though separated by 2 layers) and even if I
isolate the grounds, some noise is bound to take the signal lines.

That's one of the reasons why it's a recipe for disaster ;-)

2) Keep split power planes, but add a narrow slice ground plane
between the power plane 'fingers' in between them on the same layer as
the power planes.

Copper pour on the same plane as power? You can do that but via it
through here and there. And no thermal reliefs for those vias unless
something needs to be soldered in there.

3) Keep 1, but put connections between ground planes at regular
intervals.

That's like saying "Let's split it, oh, wait, maybe split them only a
little". I would not split the ground at all.

Anyone have thoughts on this. The voltages are +5 or less and it is
all analog..there are digital lines and a digital section, but they
come into the analog area through an isolator.

Make sure your power is clean and the switcher doesn't chatter through.
Use shielded versions for the magnetics if it's close by. Design your
stuff with reasonable PSRR or bypass extra good where you can't, like
for transistor stages.

 

[legg]

All,

I am designing a multi-channel board and I have individual linear
regulators for each channel running off a common switcher.

Now, my concern is that due to the split power planes, which are like
thin fingers running through the board, I will cause potential
differences based on the current in different channels, especially,
because I have a common ground plane. Now, I was thinking my choices
are:

1) Split the ground plane as well, so I would have thin finger like
power and ground plane separated by narrow notch but connected at the
linear regulator end and at the input end. (All the channels are w.r.t
common ground plane.)

The trouble is, that I have common (to all channels) control lines
runnning across my planes (though separated by 2 layers) and even if I
isolate the grounds, some noise is bound to take the signal lines.

2) Keep split power planes, but add a narrow slice ground plane
between the power plane 'fingers' in between them on the same layer as
the power planes.

3) Keep 1, but put connections between ground planes at regular
intervals.

Anyone have thoughts on this. The voltages are +5 or less and it is
all analog..there are digital lines and a digital section, but they
come into the analog area through an isolator.

Best just to reference and decouple the output regulators to the load
at the ground plane of the load. input decoupling will only work with
an intervening impedance at the unregulated input.

If the switcher outputs had individual returns (ie were isolated) you
might do some funny stuff with the grounds before the regulators, but
not with a common return. You might consider runnung the switcher
return to an intelligent board location, before it hits the ground
plane.

RL

 

[John Larkin]

All,

I am designing a multi-channel board and I have individual linear
regulators for each channel running off a common switcher.

Now, my concern is that due to the split power planes, which are like
thin fingers running through the board, I will cause potential
differences based on the current in different channels, especially,
because I have a common ground plane. Now, I was thinking my choices
are:

1) Split the ground plane as well, so I would have thin finger like
power and ground plane separated by narrow notch but connected at the
linear regulator end and at the input end. (All the channels are w.r.t
common ground plane.)

The trouble is, that I have common (to all channels) control lines
runnning across my planes (though separated by 2 layers) and even if I
isolate the grounds, some noise is bound to take the signal lines.

2) Keep split power planes, but add a narrow slice ground plane
between the power plane 'fingers' in between them on the same layer as
the power planes.

3) Keep 1, but put connections between ground planes at regular
intervals.

Anyone have thoughts on this. The voltages are +5 or less and it is
all analog..there are digital lines and a digital section, but they
come into the analog area through an isolator.

Keep a single, solid ground plane. Break the power plane up into
individual pours, each fed from its own regulator.

That's the best general advice I can give without getting involved in
the detailed design of your product (and you probably can't afford
me.)

John

 

[namdeguerre@gmail.com]

Splitting a ground plane is usually a recipe for disaster. I have yet to
see a case where that really worked and it's been decades now. In audio
designs it can work but only until a strong RF field shows up, upon
which all hell breaks loose.

OTOH if nobody split planes anymore I'd have less work so it does have
some upsides ;-)


That's one of the reasons why it's a recipe for disaster ;-)


Copper pour on the same plane as power? You can do that but via it
through here and there. And no thermal reliefs for those vias unless
something needs to be soldered in there.


That's like saying "Let's split it, oh, wait, maybe split them only a
little". I would not split the ground at all.


Make sure your power is clean and the switcher doesn't chatter through.
Use shielded versions for the magnetics if it's close by. Design your
stuff with reasonable PSRR or bypass extra good where you can't, like
for transistor stages.

--
Regards, Joerg

http://www.analogconsultants.com/- Hide quoted text -

- Show quoted text -

Well, actually, I am not splitting the ground planes, in the sense
that they are connected at the same potential at all the linear
regulators and at the input. But with my control lines, crossing
across my parts, my split is not going to have much effect. I could
put de-coupling caps across the notch to allow high frequencies to
pass, but again they might go through my control lines and not bother
with the caps...basically it is big ?..so yeah, I think I am not going
to split the ground...best to do it when I have free time as a test
project.

For my thin ground slice in between the power planes (on the same
layer0, I put vias every 50 mils or so and no themal reliefs and it is
a relatively unpopulated location, so that will help. My switcher and
linear regulator are LT parts 3430/1763, but I have been told by just
about every amplifier part vendor (and LT themselves!) that linear
regulators don't attenuate frequencies above 100 kHz very well, so I
might keep a 100 kHz switching frequency and maybe put ferrites at the
linear regulator input.

I am also considering using ceramic 10 uF caps instead of the tantalum
datasheets reference. Also some 0508/0402 caps.

 

[namdeguerre@gmail.com]

Best just to reference and decouple the output regulators to the load
at the ground plane of the load. input decoupling will only work with
an intervening impedance at the unregulated input.

If the switcher outputs had individual returns (ie were isolated) you
might do some funny stuff with the grounds before the regulators, but
not with a common return. You might consider runnung the switcher
return to an intelligent board location, before it hits the ground
plane.

RL- Hide quoted text -

- Show quoted text -

Unfortunately, my switcher is teh standard run of the mill, I could
use a DC-DC converter with isolation probably. My switcher return is
almost immediately goes to the ground plane as per the manufacturer
(LT) recommendation, however I can connect the grounds of the linear
regulator and the switcher to a common location and then send it to
the ground plane.

Well

 

[namdeguerre@gmail.com]

Keep a single, solid ground plane. Break the power plane up into
individual pours, each fed from its own regulator.

That's the best general advice I can give without getting involved in
the detailed design of your product (and you probably can't afford
me.)

John- Hide quoted text -

- Show quoted text -

Thanks, that is very helpful, I will stick with one plane and
hopefully the ground 'slice' between the power planes will help as
well. Also, I am wondering if putting decoupling caps between two
power plane pours will help further

 

[John Larkin]

Thanks, that is very helpful, I will stick with one plane and
hopefully the ground 'slice' between the power planes will help as
well. Also, I am wondering if putting decoupling caps between two
power plane pours will help further

Do NOT slice the ground plane. Bypass each power pour to ground.

Over and out.

John

 

[Guy Macon]

Well, actually, I am not splitting the ground planes, in the sense
that they are connected at the same potential at all the linear
regulators and at the input.

Only one of the following can be true:

[A] Your ground plane has the bare minimum of interruptions needed
to accommodate signal vias, etc., in which case you have not split
the ground plane.

you have purposely added some sort of notch, gap, hole, or
other shape of non-copper that you could have filled with copper,
in which case you have split the ground plane.

Some splits are worse than others, but case [A] is almost
always the best choice unless you are doing something really
specialized, know what you are doing, and are willing to
build and test the proposed topology to prove that case [A]
doesn't beat it. And even then case [A] tends to be better
when conditions you didn't envision arise.

I could put de-coupling caps across the notch to allow high
frequencies to pass

Replace the caps with copper (no notches). Use those caps to
bypass high frequencies your power plane(s) to your ground plane.

Unlike splitting the ground plane, having a split power plane
with separate onboard regulators for different sections is
usually a good idea, depending on your cost constraints.

My switcher and linear regulator are LT parts 3430/1763,
but I have been told by just about every amplifier part
vendor (and LT themselves!) that linear regulators don't
attenuate frequencies above 100 kHz very well,

It is always better to kill as much switching noise as
possible before feeding it into an analog regulator.

so I might keep a 100 kHz switching frequency

That's a trade-off too complex to discuss here. Higher
switcher frequencies are better at blowing past linear
regulators, jumping through the air, etc. but are easier
to kill at susceptible IC or transistor. Lower frequencies
are just the opposite.

and maybe put ferrites at the linear regulator input.

If you are building a switcher on the board, use the layout
from the app notes and data sheets for your switcher. If
it is the usual separate box, putting ferrites on the wires
is a cheap way of stopping some of the noise. Please note
that choosing ferrites and deciding where to put them is
an engineering task in itself. How big? What frequency?
Differential mode (bead per wire) or common mode (power and
return through one bigger bead)? Saturation problems?
Look for app notes that will help with those decisions.

I am also considering using ceramic 10 uF caps instead of
the tantalum datasheets reference.

Why? Do you really think that you know more than the
engineer who wrote the datasheet?

Also some 0508/0402 caps.

It is almost always a good idea to put a 0.1 ceramic
bypass cap at every power pin of every IC, depending
on your cost constraints.

For my thin ground slice in between the power planes (on the
same layer0, I put vias every 50 mils or so and no themal
reliefs and it is a relatively unpopulated location, so
that will help.

[from a later post]

Thanks, that is very helpful, I will stick with one plane and
hopefully the ground 'slice' between the power planes will help as
well.

In general, that space is better used to make the power planes
bigger.

Also, I am wondering if putting decoupling caps between two
power plane pours will help further

Not a good plan. Put those decoupling caps between each
power plane and the ground plane instead.

 

[MooseFET]

All,

I am designing a multi-channel board and I have individual linear
regulators for each channel running off a common switcher.

Now, my concern is that due to the split power planes, which are like
thin fingers running through the board, I will cause potential
differences based on the current in different channels, especially,
because I have a common ground plane. Now, I was thinking my choices
are:

1) Split the ground plane as well, so I would have thin finger like
power and ground plane separated by narrow notch but connected at the
linear regulator end and at the input end. (All the channels are w.r.t
common ground plane.)

The trouble is, that I have common (to all channels) control lines
runnning across my planes (though separated by 2 layers) and even if I
isolate the grounds, some noise is bound to take the signal lines.

2) Keep split power planes, but add a narrow slice ground plane
between the power plane 'fingers' in between them on the same layer as
the power planes.

3) Keep 1, but put connections between ground planes at regular
intervals.

4) Add yet another layer to the design. This extra layer would be the
"signal return" layer and won't carry the power currents.

 

[Joerg]

Well, actually, I am not splitting the ground planes, in the sense
that they are connected at the same potential at all the linear
regulators and at the input. But with my control lines, crossing
across my parts, my split is not going to have much effect. I could
put de-coupling caps across the notch to allow high frequencies to
pass, but again they might go through my control lines and not bother
with the caps...basically it is big ?..so yeah, I think I am not going
to split the ground...best to do it when I have free time as a test
project.

For my thin ground slice in between the power planes (on the same
layer0, I put vias every 50 mils or so and no themal reliefs and it is
a relatively unpopulated location, so that will help. My switcher and
linear regulator are LT parts 3430/1763, but I have been told by just
about every amplifier part vendor (and LT themselves!) that linear
regulators don't attenuate frequencies above 100 kHz very well, so I
might keep a 100 kHz switching frequency and maybe put ferrites at the
linear regulator input.

Easy fix if you need good rejection: Use a npn-Darlington with enough
heat dissipation capability to drop around 1.5V at your maximum current.
Collector to switcher output, emitter to linear regulator input, 1K
resistor from base to collector, 47uF cap from base to ground. Plus a
couple discharge diodes. That'll behave like having a shoe size 15
electrolytic in there.

Also, consider using the LM317. With a cap at the adjust pin it'll
maintain a low output impedance all the way up to a MHz:
http://www.national.com/ds/LM/LM117.pdf

Personally I'd resist the temptation to use an LDO. I've seen them bring
a lot of grief.

I am also considering using ceramic 10 uF caps instead of the tantalum
datasheets reference. Also some 0508/0402 caps.

Tantalums in bypass applications are quite evil IMHO. Seen too many
orange-greenish clouds wafting up after the explosion and so on.

 

[Joerg]

4) Add yet another layer to the design. This extra layer would be the
"signal return" layer and won't carry the power currents.

Careful, that can develop it's own nasty form of life. Just like a
subway station in a seedy part of town.

 

[John Larkin]

I am also considering using ceramic 10 uF caps instead of the tantalum
datasheets reference. Also some 0508/0402 caps.

Many linear regs are unstable with ceramics on the output. The
suggestion to use tantalums is their Zen way of saying so without
saying so.

John

 

[qrk]

All,

I am designing a multi-channel board and I have individual linear
regulators for each channel running off a common switcher.

Now, my concern is that due to the split power planes, which are like
thin fingers running through the board, I will cause potential
differences based on the current in different channels, especially,
because I have a common ground plane. Now, I was thinking my choices
are:

1) Split the ground plane as well, so I would have thin finger like
power and ground plane separated by narrow notch but connected at the
linear regulator end and at the input end. (All the channels are w.r.t
common ground plane.)

The trouble is, that I have common (to all channels) control lines
runnning across my planes (though separated by 2 layers) and even if I
isolate the grounds, some noise is bound to take the signal lines.

2) Keep split power planes, but add a narrow slice ground plane
between the power plane 'fingers' in between them on the same layer as
the power planes.

3) Keep 1, but put connections between ground planes at regular
intervals.

Anyone have thoughts on this. The voltages are +5 or less and it is
all analog..there are digital lines and a digital section, but they
come into the analog area through an isolator.

Keep one solid ground plane.

Using a linear regulator on each channel is a good way to isolate
power supply cross talk, so, keep that in.

You will have more problems with that switcher getting into things.
The switcher needs to be properly laid out on the pcb or you will get
switching noise into places you don't want it. Linear Tech. has the
layout of their reference designs for most or all of their switchers.
If you can't find it on LT's web site, call your LT rep. LT has
excellent customer support for the small guy. It is a good idea to use
LT's layout as a reference. If you can, use one of the MHz plus
switchers, then, apply ferrite beads to input and output of the
switcher.

 

[Joel Koltner]

Many linear regs are unstable with ceramics on the output. The
suggestion to use tantalums is their Zen way of saying so without
saying so.

It'd be handy if someone started collecting a "decoder ring" between what data
sheets say and what they really mean.

"It is suggested to use tantalum caps on the output of this regulator" -->
"This regulator is unstable with too low of ESR output caps."

Ever use chips by FTDI? They take the approach that if you want to do
something "easy" based on the register descriptions... but due to chip bugs it
doesn't actually WORK that way... they never mention there IS a bug, but
instead provide circuitous example code that works around it!

 

[Joerg]

Many linear regs are unstable with ceramics on the output. The
suggestion to use tantalums is their Zen way of saying so without
saying so.

Thou shalt not use LDOs ;-)

 

[Joel Koltner]

Thou shalt not use LDOs ;-)

Every time someone says they don't believe in LDOs a designer at Analog
Devices, Linear, or Maxim dies.

I suspect you've rolled a few discrete transistor-based LDO designs in your
time, Joerg!

 

[John Larkin]

It'd be handy if someone started collecting a "decoder ring" between what data
sheets say and what they really mean.

"It is suggested to use tantalum caps on the output of this regulator" -->
"This regulator is unstable with too low of ESR output caps."

Eventually one becomes sensitized to this sort of new-speak. Even more
fun is when you have to research the part numbers that they call out
on the eval board, because *their* esr's are the only hint about what
might work. Micrel is especially good at this trick.

Ever use chips by FTDI? They take the approach that if you want to do
something "easy" based on the register descriptions... but due to chip bugs it
doesn't actually WORK that way... they never mention there IS a bug, but
instead provide circuitous example code that works around it!

This sort of obscurity means that many, many users spend many, many
man-weeks and board spins discovering these facts over and over.

John

 

[Joerg]

Every time someone says they don't believe in LDOs a designer at Analog
Devices, Linear, or Maxim dies.

And if I'd sing my song about Maxim their CEO might clutch his chest ;-)

I suspect you've rolled a few discrete transistor-based LDO designs in your
time, Joerg!

Yes, I did. But then you know how it'll behave. Problem with modern
chips is that they don't give out much information. For example, TI
refused to release the SPICE model for one of their TPS chips after some
went unexplicably "exotherm" on our boards. They also refused to run our
simple circuitry around it. So I gave it the ax, for good. I sure won't
use one anytime soon.

 

[Joerg]

Eventually one becomes sensitized to this sort of new-speak. Even more
fun is when you have to research the part numbers that they call out
on the eval board, because *their* esr's are the only hint about what
might work. Micrel is especially good at this trick.

Even if they give you an ESR range it'll be in the figure section and
thus typical, not guaranteed. Personally I do not use LDOs with
non-guaranteed ESR ranges. Which pretty much excludes most of them. The
ones that aren't excluded (stable down to zero and stuff) are often out
of budget range.

This sort of obscurity means that many, many users spend many, many
man-weeks and board spins discovering these facts over and over.

If there is a better device from the competition just move on.