Split Ground/Power planes for sensitive analog, vs glitchy digital...

[Ricky]

I took a class many years ago, where they talked about creating separate power and ground planes for the analog and digital circuitry on a board. Of course, the ground planes would be joined at one location, typically under the chip that had both analog and digital signals, like an ADC or DAC.

The high speed digital signals would be routed anywhere other than over the analog ground planes, of course. Some people are telling me this is a bad idea, as if I have totally separate ground planes.

Any comments?

--

Rick C.

- Get 1,000 miles of free Supercharging
- Tesla referral code - https://ts.la/richard11209

 

[John Larkin]

On Sat, 22 Jul 2023 13:17:35 -0700 (PDT), Ricky
<gnuarm.deletethisbit@gmail.com> wrote:

I took a class many years ago, where they talked about creating separate power and ground planes for the analog and digital circuitry on a board. Of course, the ground planes would be joined at one location, typically under the chip that had both analog and digital signals, like an ADC or DAC.

The high speed digital signals would be routed anywhere other than over the analog ground planes, of course. Some people are telling me this is a bad idea, as if I have totally separate ground planes.

Any comments?

Almost always best is one solid ground plane for everything, bolted to
the metal case through every available spacer and bracket and
connector shell. We standardize on layer 2 for the ground plane, and
occasioanlly also layer 5 (of 6) mostly to keep the copper balanced
when we don\'t need a bunch of power planes..

Handle any microvolt ground loops properly of course.

There\'s no reason for any two grounds to be at different potentials.

The IC people think *their* single chip is the center of the universe,
and that the two system grounds should only meet under their single
chip.

 

[Lasse Langwadt Christensen]

lørdag den 22. juli 2023 kl. 22.17.42 UTC+2 skrev Ricky:

I took a class many years ago, where they talked about creating separate power and ground planes for the analog and digital circuitry on a board. Of course, the ground planes would be joined at one location, typically under the chip that had both analog and digital signals, like an ADC or DAC.

The high speed digital signals would be routed anywhere other than over the analog ground planes, of course. Some people are telling me this is a bad idea, as if I have totally separate ground planes.

Any comments?

https://resources.altium.com/p/splitting-planes-good-bad-and-ugly

 

[Ricky]

On Saturday, July 22, 2023 at 4:33:25 PM UTC-4, John Larkin wrote:

On Sat, 22 Jul 2023 13:17:35 -0700 (PDT), Ricky
gnuarm.del...@gmail.com> wrote:

I took a class many years ago, where they talked about creating separate power and ground planes for the analog and digital circuitry on a board. Of course, the ground planes would be joined at one location, typically under the chip that had both analog and digital signals, like an ADC or DAC.

The high speed digital signals would be routed anywhere other than over the analog ground planes, of course. Some people are telling me this is a bad idea, as if I have totally separate ground planes.

Any comments?
Almost always best is one solid ground plane for everything, bolted to
the metal case through every available spacer and bracket and
connector shell. We standardize on layer 2 for the ground plane, and
occasioanlly also layer 5 (of 6) mostly to keep the copper balanced
when we don\'t need a bunch of power planes..

Handle any microvolt ground loops properly of course.

There\'s no reason for any two grounds to be at different potentials.

The IC people think *their* single chip is the center of the universe,
and that the two system grounds should only meet under their single
chip.

Hmmm... Why would two ground planes be at different potentials if they are connected? Perhaps you missed where I said, \"joined at one location\".

The idea is that some circuitry, such as a switching power converter or a power hungry IC, puts large currents in the ground plane, which do not limit themselves to the immediate area under that circuit.

Connecting the two ground planes at one spot, limits the impact of these currents to the digital plane.

Of course, there is always more to a design than one such detail. This still requires the elimination of ground loops from other ground connections, such as off board.

--

Rick C.

- Get 1,000 miles of free Supercharging
- Tesla referral code - https://ts.la/richard11209

 

[Dimiter_Popoff]

On 7/22/2023 23:17, Ricky wrote:

I took a class many years ago, where they talked about creating separate power and ground planes for the analog and digital circuitry on a board. Of course, the ground planes would be joined at one location, typically under the chip that had both analog and digital signals, like an ADC or DAC.

The high speed digital signals would be routed anywhere other than over the analog ground planes, of course. Some people are telling me this is a bad idea, as if I have totally separate ground planes.

Any comments?

Just think currents. I do split planes when I have currents I don\'t
want to see go into sensitive analog areas - e.g. DC-DC converters
can be nicely contained within themselves and connect to the main
GND plane where you want their output current to go through.

Basically the rule is do it with reason, if you don\'t know why
you split a plane just don\'t, luck will likely be on your side
if you don\'t.
And of course make sure not to route fast signals across splits,
the return current flows through the plane just underneath the trace;
cut that and you have a discontinuity, potentially a killer one.

 

[Ricky]

On Saturday, July 22, 2023 at 4:38:45 PM UTC-4, Lasse Langwadt Christensen wrote:

lørdag den 22. juli 2023 kl. 22.17.42 UTC+2 skrev Ricky:
I took a class many years ago, where they talked about creating separate power and ground planes for the analog and digital circuitry on a board. Of course, the ground planes would be joined at one location, typically under the chip that had both analog and digital signals, like an ADC or DAC.

The high speed digital signals would be routed anywhere other than over the analog ground planes, of course. Some people are telling me this is a bad idea, as if I have totally separate ground planes.

Any comments?

https://resources.altium.com/p/splitting-planes-good-bad-and-ugly

There is some irony that Lee Ritchey is quoted as saying splitting of planes is always bad. That\'s who said it should be considered, in the class he taught some years ago.

One of the things in Lee\'s class that impressed me, was that nearly everything he taught he analyzed the theory, simulated and finally built boards to test the idea. That\'s very powerful evidence.

I don\'t think he built this circuit.

--

Rick C.

+ Get 1,000 miles of free Supercharging
+ Tesla referral code - https://ts.la/richard11209

 

[Ricky]

On Saturday, July 22, 2023 at 4:45:11 PM UTC-4, Dimiter_Popoff wrote:

On 7/22/2023 23:17, Ricky wrote:
I took a class many years ago, where they talked about creating separate power and ground planes for the analog and digital circuitry on a board. Of course, the ground planes would be joined at one location, typically under the chip that had both analog and digital signals, like an ADC or DAC.

The high speed digital signals would be routed anywhere other than over the analog ground planes, of course. Some people are telling me this is a bad idea, as if I have totally separate ground planes.

Any comments?

Just think currents. I do split planes when I have currents I don\'t
want to see go into sensitive analog areas - e.g. DC-DC converters
can be nicely contained within themselves and connect to the main
GND plane where you want their output current to go through.

Basically the rule is do it with reason, if you don\'t know why
you split a plane just don\'t, luck will likely be on your side
if you don\'t.
And of course make sure not to route fast signals across splits,
the return current flows through the plane just underneath the trace;
cut that and you have a discontinuity, potentially a killer one.

Yeah, people warn me about the fast digital signals all the time. I don\'t have fast digital signals in the analog circuits, only the ADC which is where the planes are split.

--

Rick C.

-- Get 1,000 miles of free Supercharging
-- Tesla referral code - https://ts.la/richard11209

 

[John Larkin]

On Sat, 22 Jul 2023 13:43:13 -0700 (PDT), Ricky
<gnuarm.deletethisbit@gmail.com> wrote:

On Saturday, July 22, 2023 at 4:33:25?PM UTC-4, John Larkin wrote:
On Sat, 22 Jul 2023 13:17:35 -0700 (PDT), Ricky
gnuarm.del...@gmail.com> wrote:

I took a class many years ago, where they talked about creating separate power and ground planes for the analog and digital circuitry on a board. Of course, the ground planes would be joined at one location, typically under the chip that had both analog and digital signals, like an ADC or DAC.

The high speed digital signals would be routed anywhere other than over the analog ground planes, of course. Some people are telling me this is a bad idea, as if I have totally separate ground planes.

Any comments?
Almost always best is one solid ground plane for everything, bolted to
the metal case through every available spacer and bracket and
connector shell. We standardize on layer 2 for the ground plane, and
occasioanlly also layer 5 (of 6) mostly to keep the copper balanced
when we don\'t need a bunch of power planes..

Handle any microvolt ground loops properly of course.

There\'s no reason for any two grounds to be at different potentials.

The IC people think *their* single chip is the center of the universe,
and that the two system grounds should only meet under their single
chip.

Hmmm... Why would two ground planes be at different potentials if they are connected? Perhaps you missed where I said, \"joined at one location\".

Don\'t be obnoxious or nobody will want to help.

One common connection location won\'t force two planes to be
equipotential, AC or DC.

I work with one giant organization whose religion includes
single-point grounding not only for multiple boards in a box, but for
entire building-sized systems. That gets absurd. Sometimes their stuff
works, typically after six iterations and three or four years.

The idea is that some circuitry, such as a switching power converter or a power hungry IC, puts large currents in the ground plane, which do not limit themselves to the immediate area under that circuit.

A dipole voltage in a plane falls off fast with distance, 3rd power as
I recall. And it\'s not hard to keep switcher currents from getting
into a ground plane.

Connecting the two ground planes at one spot, limits the impact of these currents to the digital plane.

How do you pick the \"one spot\" ?

The planes are capacitively coupled anyhow. And some power pours would
be bypassed to one plane, some to the other. Nightmare.

Of course, there is always more to a design than one such detail. This still requires the elimination of ground loops from other ground connections, such as off board.

Handle low-level signals carefully, differentially if required.

Ground planes with differential AC voltage between them cause all
sorts of problems.

The board I just posted the pic of has two reference planes, hard
ground and N, the 3-phase floating neutral. They can\'t be connected
but are mightily bypassed to one another. Some long, fast microstrip
logic signals cross the \"reference plane\" boundary.

 

[John Larkin]

On Sat, 22 Jul 2023 13:38:40 -0700 (PDT), Lasse Langwadt Christensen
<langwadt@fonz.dk> wrote:

lørdag den 22. juli 2023 kl. 22.17.42 UTC+2 skrev Ricky:
I took a class many years ago, where they talked about creating separate power and ground planes for the analog and digital circuitry on a board. Of course, the ground planes would be joined at one location, typically under the chip that had both analog and digital signals, like an ADC or DAC.

The high speed digital signals would be routed anywhere other than over the analog ground planes, of course. Some people are telling me this is a bad idea, as if I have totally separate ground planes.

Any comments?


https://resources.altium.com/p/splitting-planes-good-bad-and-ugly

\"But, perhaps one of the most important takeaways is that you should
NEVER, EVER split ground planes.\"

That\'s all you need to read.

I have a few times cut a C shape into a ground plane to create a
peninsula that is mostly free of ground loop potentials. I tucked some
nanovolt opamp circuits there. But that\'s not a separate plane and the
open side of the C only adds micro-ohms to the peninsula from the
overall plane.

 

[Joe Gwinn]

On Sat, 22 Jul 2023 23:45:00 +0300, Dimiter_Popoff <dp@tgi-sci.com>
wrote:

On 7/22/2023 23:17, Ricky wrote:
I took a class many years ago, where they talked about creating separate power and ground planes for the analog and digital circuitry on a board. Of course, the ground planes would be joined at one location, typically under the chip that had both analog and digital signals, like an ADC or DAC.

The high speed digital signals would be routed anywhere other than over the analog ground planes, of course. Some people are telling me this is a bad idea, as if I have totally separate ground planes.

Any comments?


Just think currents. I do split planes when I have currents I don\'t
want to see go into sensitive analog areas - e.g. DC-DC converters
can be nicely contained within themselves and connect to the main
GND plane where you want their output current to go through.

Basically the rule is do it with reason, if you don\'t know why
you split a plane just don\'t, luck will likely be on your side
if you don\'t.
And of course make sure not to route fast signals across splits,
the return current flows through the plane just underneath the trace;
cut that and you have a discontinuity, potentially a killer one.

There are lots of reasons to have separate ground planes. The classic
is to separate digital from analog circuitry, as digital can be pretty
noisy, and analog can interpret ground bounce as a valid input.

Another reason to have multiple analog ground planes is a Dual Mixer
Time Difference instrument, where the beatnote between ~ 10 MHz
carriers is one to ten Hertz, so the \"just underneath the trace\" fills
the entire ground plane uniformly. The usual dodge is to
transformer-couple the two RF carriers, generating the sinewave
beatnote with a double-balanced diode-ring mixer on the floating
ground plane, and transmit the beatnote signal differentially over
shielded twisted pair cable to where it will be used, or to square the
beatnote sinewave and send that by shielded twisted pair cable.

The classic reference is \"Noise Reduction Techniques in Electronic
Systems\", 2nd Edition, by Henry W. Ott, Wiley 1988, 448 pages.

..<https://www.amazon.com/Noise-Reduction-Techniques-Electronic-Systems/dp/0471850683>

Also covered in \"Electromagnetic Compatibility Engineering First
Edition\", also by Ott, Wiley 2009, 880 pages.

..<https://www.amazon.com/Electromagnetic-Compatibility-Engineering-Henry-Ott/dp/0470189304>


Joe Gwinn

 

[John Larkin]

On Sat, 22 Jul 2023 23:45:00 +0300, Dimiter_Popoff <dp@tgi-sci.com>
wrote:

On 7/22/2023 23:17, Ricky wrote:
I took a class many years ago, where they talked about creating separate power and ground planes for the analog and digital circuitry on a board. Of course, the ground planes would be joined at one location, typically under the chip that had both analog and digital signals, like an ADC or DAC.

The high speed digital signals would be routed anywhere other than over the analog ground planes, of course. Some people are telling me this is a bad idea, as if I have totally separate ground planes.

Any comments?


Just think currents. I do split planes when I have currents I don\'t
want to see go into sensitive analog areas - e.g. DC-DC converters
can be nicely contained within themselves and connect to the main
GND plane where you want their output current to go through.

Basically the rule is do it with reason, if you don\'t know why
you split a plane just don\'t, luck will likely be on your side
if you don\'t.
And of course make sure not to route fast signals across splits,
the return current flows through the plane just underneath the trace;
cut that and you have a discontinuity, potentially a killer one.

I\'ve TDR tested microstrips that cross ground splits or cuts, or
transition from running over a ground to over a power pour. At 30 pS
resolution, the crossing is generally invisible.

In a multilayer board, plane-plane capacitance is high so a trace
doesn\'t notice changing reference planes. AC-wise, the board is a
monolithic equipotential brick.

Hard right angles are usually TDR invisible too, or so small a
discontinuity that few signals would care.

There\'s a lot of folklore in PCB design.

 

[Dimiter_Popoff]

On 7/23/2023 0:39, John Larkin wrote:

On Sat, 22 Jul 2023 23:45:00 +0300, Dimiter_Popoff <dp@tgi-sci.com
wrote:

On 7/22/2023 23:17, Ricky wrote:
I took a class many years ago, where they talked about creating separate power and ground planes for the analog and digital circuitry on a board. Of course, the ground planes would be joined at one location, typically under the chip that had both analog and digital signals, like an ADC or DAC.

The high speed digital signals would be routed anywhere other than over the analog ground planes, of course. Some people are telling me this is a bad idea, as if I have totally separate ground planes.

Any comments?


Just think currents. I do split planes when I have currents I don\'t
want to see go into sensitive analog areas - e.g. DC-DC converters
can be nicely contained within themselves and connect to the main
GND plane where you want their output current to go through.

Basically the rule is do it with reason, if you don\'t know why
you split a plane just don\'t, luck will likely be on your side
if you don\'t.
And of course make sure not to route fast signals across splits,
the return current flows through the plane just underneath the trace;
cut that and you have a discontinuity, potentially a killer one.

I\'ve TDR tested microstrips that cross ground splits or cuts, or
transition from running over a ground to over a power pour. At 30 pS
resolution, the crossing is generally invisible.

How close to the discontinued plane was the next one the signal
would have gone through?

In a multilayer board, plane-plane capacitance is high so a trace
doesn\'t notice changing reference planes. AC-wise, the board is a
monolithic equipotential brick.

Well unless the alternate plane is far enough (say 1mm). But I guess
you are talking multiple layers, 0.1mm or so separation, which I
can believe (have not done that sort of test).

Hard right angles are usually TDR invisible too, or so small a
discontinuity that few signals would care.

There\'s a lot of folklore in PCB design.

Hard right angles sound more like folklore, I can understand how
some signals could care (not experienced any of it though).

 

[Dimiter_Popoff]

On 7/23/2023 0:36, Joe Gwinn wrote:

On Sat, 22 Jul 2023 23:45:00 +0300, Dimiter_Popoff <dp@tgi-sci.com
wrote:

On 7/22/2023 23:17, Ricky wrote:
I took a class many years ago, where they talked about creating separate power and ground planes for the analog and digital circuitry on a board. Of course, the ground planes would be joined at one location, typically under the chip that had both analog and digital signals, like an ADC or DAC.

The high speed digital signals would be routed anywhere other than over the analog ground planes, of course. Some people are telling me this is a bad idea, as if I have totally separate ground planes.

Any comments?


Just think currents. I do split planes when I have currents I don\'t
want to see go into sensitive analog areas - e.g. DC-DC converters
can be nicely contained within themselves and connect to the main
GND plane where you want their output current to go through.

Basically the rule is do it with reason, if you don\'t know why
you split a plane just don\'t, luck will likely be on your side
if you don\'t.
And of course make sure not to route fast signals across splits,
the return current flows through the plane just underneath the trace;
cut that and you have a discontinuity, potentially a killer one.

There are lots of reasons to have separate ground planes. The classic
is to separate digital from analog circuitry, as digital can be pretty
noisy, and analog can interpret ground bounce as a valid input.

Another reason to have multiple analog ground planes is a Dual Mixer
Time Difference instrument, where the beatnote between ~ 10 MHz
carriers is one to ten Hertz, so the \"just underneath the trace\" fills
the entire ground plane uniformly. The usual dodge is to
transformer-couple the two RF carriers, generating the sinewave
beatnote with a double-balanced diode-ring mixer on the floating
ground plane, and transmit the beatnote signal differentially over
shielded twisted pair cable to where it will be used, or to square the
beatnote sinewave and send that by shielded twisted pair cable.

The classic reference is \"Noise Reduction Techniques in Electronic
Systems\", 2nd Edition, by Henry W. Ott, Wiley 1988, 448 pages.

.<https://www.amazon.com/Noise-Reduction-Techniques-Electronic-Systems/dp/0471850683

Also covered in \"Electromagnetic Compatibility Engineering First
Edition\", also by Ott, Wiley 2009, 880 pages.

.<https://www.amazon.com/Electromagnetic-Compatibility-Engineering-Henry-Ott/dp/0470189304


Joe Gwinn

I am not an RF person, I mostly think time domain so I am not
sure I understand all of what you say.
That very low frequency thing must be quite juicy in order to
make a difference, or (and?) you must have some very sensitive
stuff to be affected.
>

 

[John Larkin]

On Sun, 23 Jul 2023 00:59:00 +0300, Dimiter_Popoff <dp@tgi-sci.com>
wrote:

On 7/23/2023 0:39, John Larkin wrote:
On Sat, 22 Jul 2023 23:45:00 +0300, Dimiter_Popoff <dp@tgi-sci.com
wrote:

On 7/22/2023 23:17, Ricky wrote:
I took a class many years ago, where they talked about creating separate power and ground planes for the analog and digital circuitry on a board. Of course, the ground planes would be joined at one location, typically under the chip that had both analog and digital signals, like an ADC or DAC.

The high speed digital signals would be routed anywhere other than over the analog ground planes, of course. Some people are telling me this is a bad idea, as if I have totally separate ground planes.

Any comments?


Just think currents. I do split planes when I have currents I don\'t
want to see go into sensitive analog areas - e.g. DC-DC converters
can be nicely contained within themselves and connect to the main
GND plane where you want their output current to go through.

Basically the rule is do it with reason, if you don\'t know why
you split a plane just don\'t, luck will likely be on your side
if you don\'t.
And of course make sure not to route fast signals across splits,
the return current flows through the plane just underneath the trace;
cut that and you have a discontinuity, potentially a killer one.

I\'ve TDR tested microstrips that cross ground splits or cuts, or
transition from running over a ground to over a power pour. At 30 pS
resolution, the crossing is generally invisible.

How close to the discontinued plane was the next one the signal
would have gone through?

I tried one case with a 50 ohm microstrip, about 50 mils wide,
crossing a cut in the layer-2 ground plane about 20 mils wide. The
trace, looking down, sees a slightly higher capacitance where there is
a gap in the metal and epoxy is visible through that gap. As I recall,
the discontinuity was questionally visible among the usual trace
woopie-doos.

Of course both sides of the cut were equipotential, and that plane was
parallel to another unbroken plane, so plane-plane capacitances glues
everything together.

There could in theory be a slotline resonance at a slit in a ground
plane, but I\'ve never seen any evidence of that in a TDR.

We often have a trace swap its \"reference\" between different pour pour
regions, and that seems to always work.

The \"return current\" concept usually makes no sense. Just keep all the
planes parallel and reasonably bypassed, and traces will be happy
riding over any of them.

In a multilayer board, plane-plane capacitance is high so a trace
doesn\'t notice changing reference planes. AC-wise, the board is a
monolithic equipotential brick.

Well unless the alternate plane is far enough (say 1mm). But I guess
you are talking multiple layers, 0.1mm or so separation, which I
can believe (have not done that sort of test).

Our most common board is 6 layers with roughly equal gaps between
planes, of maybe a lottle closer between grounds and power planes.

We try to keep the stack symmetric and pours all over planes to
minimize board warping.

Hard right angles are usually TDR invisible too, or so small a
discontinuity that few signals would care.

There\'s a lot of folklore in PCB design.


Hard right angles sound more like folklore, I can understand how
some signals could care (not experienced any of it though).

The classic Motorola ECL Handbook cautioned about right angles, when
ECL was still 1 ns stuff at best.

Few signals are fast enough to care about even 1\"-scale abberations.

Our fastest signals are in the 40 ps range, and vias are the worst
features. Best to have none in the critical signal paths.

 

[Joe Gwinn]

On Sun, 23 Jul 2023 01:02:37 +0300, Dimiter_Popoff <dp@tgi-sci.com>
wrote:

On 7/23/2023 0:36, Joe Gwinn wrote:
On Sat, 22 Jul 2023 23:45:00 +0300, Dimiter_Popoff <dp@tgi-sci.com
wrote:

On 7/22/2023 23:17, Ricky wrote:
I took a class many years ago, where they talked about creating separate power and ground planes for the analog and digital circuitry on a board. Of course, the ground planes would be joined at one location, typically under the chip that had both analog and digital signals, like an ADC or DAC.

The high speed digital signals would be routed anywhere other than over the analog ground planes, of course. Some people are telling me this is a bad idea, as if I have totally separate ground planes.

Any comments?


Just think currents. I do split planes when I have currents I don\'t
want to see go into sensitive analog areas - e.g. DC-DC converters
can be nicely contained within themselves and connect to the main
GND plane where you want their output current to go through.

Basically the rule is do it with reason, if you don\'t know why
you split a plane just don\'t, luck will likely be on your side
if you don\'t.
And of course make sure not to route fast signals across splits,
the return current flows through the plane just underneath the trace;
cut that and you have a discontinuity, potentially a killer one.

There are lots of reasons to have separate ground planes. The classic
is to separate digital from analog circuitry, as digital can be pretty
noisy, and analog can interpret ground bounce as a valid input.

Another reason to have multiple analog ground planes is a Dual Mixer
Time Difference instrument, where the beatnote between ~ 10 MHz
carriers is one to ten Hertz, so the \"just underneath the trace\" fills
the entire ground plane uniformly. The usual dodge is to
transformer-couple the two RF carriers, generating the sinewave
beatnote with a double-balanced diode-ring mixer on the floating
ground plane, and transmit the beatnote signal differentially over
shielded twisted pair cable to where it will be used, or to square the
beatnote sinewave and send that by shielded twisted pair cable.

The classic reference is \"Noise Reduction Techniques in Electronic
Systems\", 2nd Edition, by Henry W. Ott, Wiley 1988, 448 pages.

.<https://www.amazon.com/Noise-Reduction-Techniques-Electronic-Systems/dp/0471850683

Also covered in \"Electromagnetic Compatibility Engineering First
Edition\", also by Ott, Wiley 2009, 880 pages.

.<https://www.amazon.com/Electromagnetic-Compatibility-Engineering-Henry-Ott/dp/0470189304


Joe Gwinn

I am not an RF person, I mostly think time domain so I am not
sure I understand all of what you say.
That very low frequency thing must be quite juicy in order to
make a difference, or (and?) you must have some very sensitive
stuff to be affected.

The Dual Mixer Time Difference (DMTD) instruments are used to measure
low frequency instability of clock oscillators, for Allan Deviation
(ADEV) levels below 10^-14. So it does see all manner of stuff.

For background, look it up here:

..<https://www.nist.gov/pml/time-and-frequency-division/popular-links/time-frequency-z/time-and-frequency-z-d>

Joe Gwinn

 

[Ricky]

On Saturday, July 22, 2023 at 5:21:31 PM UTC-4, John Larkin wrote:

On Sat, 22 Jul 2023 13:43:13 -0700 (PDT), Ricky
gnuarm.del...@gmail.com> wrote:
On Saturday, July 22, 2023 at 4:33:25?PM UTC-4, John Larkin wrote:
On Sat, 22 Jul 2023 13:17:35 -0700 (PDT), Ricky
gnuarm.del...@gmail.com> wrote:

I took a class many years ago, where they talked about creating separate power and ground planes for the analog and digital circuitry on a board.. Of course, the ground planes would be joined at one location, typically under the chip that had both analog and digital signals, like an ADC or DAC.

The high speed digital signals would be routed anywhere other than over the analog ground planes, of course. Some people are telling me this is a bad idea, as if I have totally separate ground planes.

Any comments?
Almost always best is one solid ground plane for everything, bolted to
the metal case through every available spacer and bracket and
connector shell. We standardize on layer 2 for the ground plane, and
occasioanlly also layer 5 (of 6) mostly to keep the copper balanced
when we don\'t need a bunch of power planes..

Handle any microvolt ground loops properly of course.

There\'s no reason for any two grounds to be at different potentials.

The IC people think *their* single chip is the center of the universe,
and that the two system grounds should only meet under their single
chip.

Hmmm... Why would two ground planes be at different potentials if they are connected? Perhaps you missed where I said, \"joined at one location\".
Don\'t be obnoxious or nobody will want to help.

I don\'t expect to hear from you. You have often said I\'m in your killfile list. Please return me there if you don\'t like what I post.

One common connection location won\'t force two planes to be
equipotential, AC or DC.

That\'s only an issue if there is significant current flowing through the connection. Why would there be significant current flowing from the sensitive analog circuits to the digital circuits. You have to do more than just connect the two areas at one point. You have to pay attention to the entire grounding plan. But there\'s nothing inherently bad about making such a connection to keep digital and switcher currents out of the analog circuits.

I work with one giant organization whose religion includes
single-point grounding not only for multiple boards in a box, but for
entire building-sized systems. That gets absurd. Sometimes their stuff
works, typically after six iterations and three or four years.

The idea is that some circuitry, such as a switching power converter or a power hungry IC, puts large currents in the ground plane, which do not limit themselves to the immediate area under that circuit.
A dipole voltage in a plane falls off fast with distance, 3rd power as
I recall. And it\'s not hard to keep switcher currents from getting
into a ground plane.

You mean like isolating the ground plane under the switcher circuit, connected at one point to the rest of the ground plane? I think that might just work. Thanks for recommending it.

Connecting the two ground planes at one spot, limits the impact of these currents to the digital plane.
How do you pick the \"one spot\" ?

For an ADC circuit, the ADC is typically a good point. The high speed digital signals get a digital ground plane, and the analog circuit gets an analog plane, with very little voltage between the two, not that this matters. What matters is keeping currents out of the analog plane, so there isn\'t digital noise in the analog plane, showing up in the analog signals.

The planes are capacitively coupled anyhow. And some power pours would
be bypassed to one plane, some to the other. Nightmare.

LOL How would two separated areas on a ground layer, be capacitively coupled??? I don\'t know what you are talking about here.

Yes, all the power rails have their own power planes. They capacitively couple to the appropriate ground plane area.

Of course, there is always more to a design than one such detail. This still requires the elimination of ground loops from other ground connections, such as off board.
Handle low-level signals carefully, differentially if required.

Or... just don\'t inject noise from the digital circuits.

Ground planes with differential AC voltage between them cause all
sorts of problems.

Yes, that would be terrible. That\'s why they need to be connected. But the voltage between the ground plane areas is not so important, as long as it is within the tolerance of the devices spanning the two plane areas. I can\'t think of a reason why, a connection with very little current flowing through it, would produce much of a voltage offset. Can you? I suppose you have some experience with this.

My designs are always pretty simple, because I try hard to not let them get difficult, like designing differential circuits to minimize the impact of noise that I didn\'t need to introduce in the first place.

Was that polite enough?

--

Rick C.

-+ Get 1,000 miles of free Supercharging
-+ Tesla referral code - https://ts.la/richard11209

 

[Ricky]

On Saturday, July 22, 2023 at 5:29:17 PM UTC-4, John Larkin wrote:

On Sat, 22 Jul 2023 13:38:40 -0700 (PDT), Lasse Langwadt Christensen
lang...@fonz.dk> wrote:

lørdag den 22. juli 2023 kl. 22.17.42 UTC+2 skrev Ricky:
I took a class many years ago, where they talked about creating separate power and ground planes for the analog and digital circuitry on a board. Of course, the ground planes would be joined at one location, typically under the chip that had both analog and digital signals, like an ADC or DAC.

The high speed digital signals would be routed anywhere other than over the analog ground planes, of course. Some people are telling me this is a bad idea, as if I have totally separate ground planes.

Any comments?


https://resources.altium.com/p/splitting-planes-good-bad-and-ugly

\"But, perhaps one of the most important takeaways is that you should
NEVER, EVER split ground planes.\"

That\'s all you need to read.

I don\'t split ground planes. I keep them separate, tied at one point.

I have a few times cut a C shape into a ground plane to create a
peninsula that is mostly free of ground loop potentials. I tucked some
nanovolt opamp circuits there. But that\'s not a separate plane and the
open side of the C only adds micro-ohms to the peninsula from the
overall plane.

Ah, so you agree with the split, but connected plane concept! Thanks. I appreciate the support. Now, we just need to work out how much connectivity is required.

How much current flowed between the two ground plane areas?

--

Rick C.

+- Get 1,000 miles of free Supercharging
+- Tesla referral code - https://ts.la/richard11209

 

[Ricky]

On Saturday, July 22, 2023 at 5:59:09 PM UTC-4, Dimiter_Popoff wrote:

On 7/23/2023 0:39, John Larkin wrote:
On Sat, 22 Jul 2023 23:45:00 +0300, Dimiter_Popoff <d...@tgi-sci.com
wrote:

On 7/22/2023 23:17, Ricky wrote:
I took a class many years ago, where they talked about creating separate power and ground planes for the analog and digital circuitry on a board.. Of course, the ground planes would be joined at one location, typically under the chip that had both analog and digital signals, like an ADC or DAC.

The high speed digital signals would be routed anywhere other than over the analog ground planes, of course. Some people are telling me this is a bad idea, as if I have totally separate ground planes.

Any comments?


Just think currents. I do split planes when I have currents I don\'t
want to see go into sensitive analog areas - e.g. DC-DC converters
can be nicely contained within themselves and connect to the main
GND plane where you want their output current to go through.

Basically the rule is do it with reason, if you don\'t know why
you split a plane just don\'t, luck will likely be on your side
if you don\'t.
And of course make sure not to route fast signals across splits,
the return current flows through the plane just underneath the trace;
cut that and you have a discontinuity, potentially a killer one.

I\'ve TDR tested microstrips that cross ground splits or cuts, or
transition from running over a ground to over a power pour. At 30 pS
resolution, the crossing is generally invisible.
How close to the discontinued plane was the next one the signal
would have gone through?

In a multilayer board, plane-plane capacitance is high so a trace
doesn\'t notice changing reference planes. AC-wise, the board is a
monolithic equipotential brick.
Well unless the alternate plane is far enough (say 1mm). But I guess
you are talking multiple layers, 0.1mm or so separation, which I
can believe (have not done that sort of test).

Hard right angles are usually TDR invisible too, or so small a
discontinuity that few signals would care.

There\'s a lot of folklore in PCB design.

Hard right angles sound more like folklore, I can understand how
some signals could care (not experienced any of it though).

The right angle trace effect is real, but people often use the wrong explanation, such as \"the signal flying off the end of the wire, rather than making the turn\" (I\'ve actually had someone tell me that with a straight face). The simple fact is that the corner represents a lumped capacitance in the trace. Often, that is of no consequence. Sometimes it is of consequence. Depends on all the many details.

Rounding the corner makes the lumped capacitance a much, much lower value to the point of vanishing. Making it a pair of 45 degree bends does a pretty good job too.

--

Rick C.

++ Get 1,000 miles of free Supercharging
++ Tesla referral code - https://ts.la/richard11209

 

[Don]

Joe Gwinn wrote:

<snip>

There are lots of reasons to have separate ground planes. The classic
is to separate digital from analog circuitry, as digital can be pretty
noisy, and analog can interpret ground bounce as a valid input.

Another reason to have multiple analog ground planes is a Dual Mixer
Time Difference instrument, where the beatnote between ~ 10 MHz
carriers is one to ten Hertz, so the \"just underneath the trace\" fills
the entire ground plane uniformly. The usual dodge is to
transformer-couple the two RF carriers, generating the sinewave
beatnote with a double-balanced diode-ring mixer on the floating
ground plane, and transmit the beatnote signal differentially over
shielded twisted pair cable to where it will be used, or to square the
beatnote sinewave and send that by shielded twisted pair cable.

The classic reference is \"Noise Reduction Techniques in Electronic
Systems\", 2nd Edition, by Henry W. Ott, Wiley 1988, 448 pages.

.<https://www.amazon.com/Noise-Reduction-Techniques-Electronic-Systems/dp
/0471850683

Also covered in \"Electromagnetic Compatibility Engineering First
Also covered in \"Electromagnetic Compatibility Engineering First
Edition\", also by Ott, Wiley 2009, 880 pages.

.<https://www.amazon.com/Electromagnetic-Compatibility-Engineering-Henry-Ott/dp/0470189304

In the case of complex RF circuits, the _ARRL Handbook_ advises against
single point grounding. Instead it suggests breaking a unit into
modules, each with its own full copper ground plane, connected by coax
to other modules.
Elecraft <https://elecraft.com/> follows this approach. And also
enjoys wildly successful products.

Danke,

--
Don, KB7RPU, https://www.qsl.net/kb7rpu
There was a young lady named Bright Whose speed was far faster than light;
She set out one day In a relative way And returned on the previous night.

 

[Anthony William Sloman]

On Sunday, July 23, 2023 at 7:21:31 AM UTC+10, John Larkin wrote:

On Sat, 22 Jul 2023 13:43:13 -0700 (PDT), Ricky
gnuarm.del...@gmail.com> wrote:
On Saturday, July 22, 2023 at 4:33:25?PM UTC-4, John Larkin wrote:
On Sat, 22 Jul 2023 13:17:35 -0700 (PDT), Ricky
gnuarm.del...@gmail.com> wrote:

I took a class many years ago, where they talked about creating separate power and ground planes for the analog and digital circuitry on a board.. Of course, the ground planes would be joined at one location, typically under the chip that had both analog and digital signals, like an ADC or DAC.

The high speed digital signals would be routed anywhere other than over the analog ground planes, of course. Some people are telling me this is a bad idea, as if I have totally separate ground planes.

Any comments?

Almost always best is one solid ground plane for everything, bolted to
the metal case through every available spacer and bracket and
connector shell. We standardize on layer 2 for the ground plane, and
occasionally also layer 5 (of 6) mostly to keep the copper balanced
when we don\'t need a bunch of power planes..

Handle any microvolt ground loops properly of course.

There\'s no reason for any two grounds to be at different potentials.

It there\'s current flowing through either of them. there\'s a [potential drop along the current path.

The IC people think *their* single chip is the center of the universe, and that the two system grounds should only meet under their single chip.

Hmmm... Why would two ground planes be at different potentials if they are connected? Perhaps you missed where I said, \"joined at one location\".

Don\'t be obnoxious or nobody will want to help.

It\'s a legitimate question. The non-obnoxious response would have been to draw his attention the fact there there\'s always a voltage drop along a current path.

I do dream of super-conducting ground planes, but they are probably a long way off.

One common connection location won\'t force two planes to be equipotential, AC or DC.

But close to it.

> I work with one giant organization whose religion includes single-point grounding not only for multiple boards in a box, but for entire building-sized systems. That gets absurd. Sometimes their stuff works, typically after six iterations and three or four years.

Complicated systems take time to get right.

The idea is that some circuitry, such as a switching power converter or a power hungry IC, puts large currents in the ground plane, which do not limit themselves to the immediate area under that circuit.

A dipole voltage in a plane falls off fast with distance, 3rd power as I recall. And it\'s not hard to keep switcher currents from getting into a ground plane.

But it does take attention.

Connecting the two ground planes at one spot, limits the impact of these currents to the digital plane.

How do you pick the \"one spot\" ?

Very carefully.

> The planes are capacitively coupled anyhow. And some power pours would be bypassed to one plane, some to the other. Nightmare.

Not if you think about what you are doing. And screening plane can greatly reduced cross-talk. Ralph Morrison\'s \"Grounding and Shielding Techniques in Instrumentation\"

https://www.amazon.com.au/Grounding-Shielding-Techniques-Instrumentation-Morrison/dp/0471838055

talked about double screening transformers forty years ago.

Of course, there is always more to a design than one such detail. This still requires the elimination of ground loops from other ground connections, such as off board.
Handle low-level signals carefully, differentially if required.

Ground planes with differential AC voltage between them cause all sorts of problems.

Fewer if you know what you are doing.

The board I just posted the pic of has two reference planes, hard
ground and N, the 3-phase floating neutral. They can\'t be connected
but are mightily bypassed to one another. Some long, fast microstrip
logic signals cross the \"reference plane\" boundary.

Not a good idea. The fast current in the microstrip needs to be balanced by the return current in the ground plane. If the return current has to make an excursion you see a discontinuity, and get reflections.

--
Bill Sloman, Sydney