Maker Pro
Maker Pro

Mixed-signal RF grounding

T

Tom Derham

Jan 1, 1970
0
Despite having read a number of books on high speed circuit design, I am
still somewhat confused as to the recommended approach, so would appreciate
some advice.

I have several high speed (100MHz clock) digital (DSP, FPGA), mixed signal
(ADC, DDS) and pure analog microwave boards (PLL, microwave amplifiers at
2.4GHz).
I can choose whether or not to have split grounds on the mixed signal boards
as I am designing them. All boards are mounted in a metal chassis, but I
can choose whether or not to isolate the grounded mounting holes on the
boards to the chassis mountings.

I know that star grounding is ineffective at high frequencies due to the
inductance of the cables, yet generally single-point grounding is advocated
to prevent unpredictable current flow in the chassis. Generally it is
advised to have separate analog and digital ground planes and connect them
in only one location (the power supply).
But if I do this, and use the chassis just as the analog ground, and isolate
the digital ground completely except for one connection at the PSU, is it ok
to use star grounding for the digital ground between the boards?
Also if grounds are completely isolated on individual boards, then won't
that make the EMI radiation bad, because (for example) power traces on the
board that cross the boundary between the two grounds will have no direct
current return path, except via the power supply connection.

Any thoughts would be most appreciated

Tom
 
J

Joerg

Jan 1, 1970
0
Hi Tom,

One low impedance common ground plane is how I design stuff. Split
grounds are treacherous. You never know whether a split is a true split.
Just think about the impedance of a stray capacitance across two planes
of, say, 20pF at a few hundred MHz. That's how high you have to go since
100MHz clocks mean rise times of a nanosecond or so.

I know that split grounds are widely touted in literature, universities,
even app notes. But they have brought me a lot of work when it turned
out that clients couldn't make it reliable.

A common ground does not relieve us from figuring the optimal placement
of circuit sections. For example, it won't exactly help if a 2.4GHz
final amp sits next to a clock generator for the ADCs. In the same way
you should not have a memory bank sloshing several amps on VCC and GND
at the far end from the supply connection. But I assume you are familiar
with that stuff. In case you do get into trouble I am sure you could
line up consulting help in this forum :).

The only exception I make from the common ground approach is in
situations where you must be isolated. An example is a patient interface
for med equipment where the rules say that the patient side has to be
completely floating and sometimes even has to withstand a blow of around
5KV. Such as in a case when the patient is being defibrillated in an
emergency situation and chances are the cables will not be disconnected
as prescribed. There are many other areas where this applies, aircraft
gear, mining equipment, powerline diagnosis and so on.

Regards, Joerg
 
J

John Larkin

Jan 1, 1970
0
Despite having read a number of books on high speed circuit design, I am
still somewhat confused as to the recommended approach, so would appreciate
some advice.

I have several high speed (100MHz clock) digital (DSP, FPGA), mixed signal
(ADC, DDS) and pure analog microwave boards (PLL, microwave amplifiers at
2.4GHz).
I can choose whether or not to have split grounds on the mixed signal boards
as I am designing them.
Don't.


All boards are mounted in a metal chassis, but I
can choose whether or not to isolate the grounded mounting holes on the
boards to the chassis mountings.

Don't.

I know that star grounding is ineffective at high frequencies due to the
inductance of the cables, yet generally single-point grounding is advocated
to prevent unpredictable current flow in the chassis. Generally it is
advised to have separate analog and digital ground planes and connect them
in only one location (the power supply).

At high frequencies, that's absurd. The various "grounds" will be
flailing all over the place relative to each other, the box, and the
outside world.
But if I do this, and use the chassis just as the analog ground, and isolate
the digital ground completely except for one connection at the PSU, is it ok
to use star grounding for the digital ground between the boards?
Also if grounds are completely isolated on individual boards, then won't
that make the EMI radiation bad, because (for example) power traces on the
board that cross the boundary between the two grounds will have no direct
current return path, except via the power supply connection.

Any thoughts would be most appreciated

Tom

Use a single PCB ground plane, and bolt it to the chassis as many
places as you can. Handle low-level problems locally.

John
 
J

Joerg

Jan 1, 1970
0
Use a single PCB ground plane, and bolt it to the chassis as many
places as you can. Handle low-level problems locally.

John
Way to go, John. But if everybody did that my business would be
shrinking :-(.

Regards, Joerg
 
J

John Larkin

Jan 1, 1970
0
Way to go, John. But if everybody did that my business would be
shrinking :-(.

Regards, Joerg


Oops, sorry. But I'll never convince them, so your revenue stream
continues.

John
 
K

Kevin Aylward

Jan 1, 1970
0
John said:
At high frequencies, that's absurd. The various "grounds" will be
flailing all over the place relative to each other, the box, and the
outside world.

Don't use ground at all for signals. Make the interface differential.
Use a single PCB ground plane, and bolt it to the chassis as many
places as you can.
Maybe.

Handle low-level problems locally.
Yes.


John

I don't like connecting everything to ground, certainly I don't like
connecting everything to chassis willy nilly. When you do this, despite
claimed low impedance ground planes, they aint. The only way to know
and control where signals flow, is to know and control where signals
flow.

You need to connect each type of signal the right way. Some will be ok
connected to chassis as much as possible, some won't. For example, in
audio mixers, *never* do it.

Keep all communication between boards differential. For *low* level
analog have lots of *local*
star points for signals that are related to each other, do not connect
them to any old point on the ground plane. Its simple to see why. Make a
spice setup of a few nh in series to mimic a ground plane, and some
others to mimic a power place, with cap decoupling with esr and esl
between them. Now switch *only* 10ma at 5ns on the chain somewhere and
actually
*look* at the levels on the "ground" chain of inductors. If your
processing uV, MHz, signals, your fucked. Actually, even mv signals and
your fucked.

e.g. I just knocked up a little 3 series 3nh chain. Switching 5 V/5ns at
500
ohms, gives say, 5mv pulses, with 1 mv across a "ground" chain.
Therefore, processing such signals *requires* a centre point. The can't
be *any* common mode impedance. I have actually done this successfully
for ultrasound where the effective input noise was at the 1 uv mark at
10Mhz, with loads of digital switching on the same board.

Kevin Aylward
[email protected]
http://www.anasoft.co.uk
SuperSpice, a very affordable Mixed-Mode
Windows Simulator with Schematic Capture,
Waveform Display, FFT's and Filter Design.
 
T

Tom Derham

Jan 1, 1970
0
Therefore, processing such signals *requires* a centre point. The can't
be *any* common mode impedance. I have actually done this successfully
for ultrasound where the effective input noise was at the 1 uv mark at
10Mhz, with loads of digital switching on the same board.

Thanks for the replies - very useful.
So on that basis, should a chain of microwave components (e.g.
SMA-connectorised low noise amplifier, filters, mixers) be individually
bolted to the chassis, or mounted to their own plate which is connected at a
single point to the chassis, or something different?

Thanks

Tom
 
J

Jamie

Jan 1, 1970
0
i like shielded grounds my self, they have solved toons of problems for me..
using coax, join the shield and center conductor together to the
ground point and center conductor only to the chassis.
you get your electrical ground but helps stop skin effects that take
place in high R.F. invironments.. event helps stop man man noise from
coming into the receivers in cases of long ground runs.
 
J

Joerg

Jan 1, 1970
0
Hi Tom,
If it was my project I'd start with bolting them all down. But make sure the materials are compatible and conductive, meaning none of this fancy anodized aluminum. Looks great but usually the surface doesn't conduct. Although for microwave the capacitance of a bolted-down surface might be enough.

At 2.4GHz a star ground is pretty meaningless. Anything past an inch or so would be a huge inductor here.

Regards, Joerg
 
R

Rene Tschaggelar

Jan 1, 1970
0
Tom said:
Despite having read a number of books on high speed circuit design, I am
still somewhat confused as to the recommended approach, so would appreciate
some advice.

I have several high speed (100MHz clock) digital (DSP, FPGA), mixed signal
(ADC, DDS) and pure analog microwave boards (PLL, microwave amplifiers at
2.4GHz).
I can choose whether or not to have split grounds on the mixed signal boards
as I am designing them. All boards are mounted in a metal chassis, but I
can choose whether or not to isolate the grounded mounting holes on the
boards to the chassis mountings.

I know that star grounding is ineffective at high frequencies due to the
inductance of the cables, yet generally single-point grounding is advocated
to prevent unpredictable current flow in the chassis. Generally it is
advised to have separate analog and digital ground planes and connect them
in only one location (the power supply).
But if I do this, and use the chassis just as the analog ground, and isolate
the digital ground completely except for one connection at the PSU, is it ok
to use star grounding for the digital ground between the boards?
Also if grounds are completely isolated on individual boards, then won't
that make the EMI radiation bad, because (for example) power traces on the
board that cross the boundary between the two grounds will have no direct
current return path, except via the power supply connection.


I'm having similar problems with mixed signal boards.
Having everything on one groupd plane is not useable since
the high frequency is everywhere. And having switchmode
power supply noise is especially bad. Not much better are the
fast FPGA and CPU signals. They have to be confined.

The high frequency part requires a GND plane, and possibly having
empty spaces on top with a GND plane too bolted down.
The control and monitor signals from the RF part to the sensitive
analog part ougth to be filtered with ferrites and caps forming a Pi or
T, depending on the impedance.
Digital signals from the digital part tend to have a lot of noise
on them and require filtering down to the required bandwidth.
The digital part also requires an own GND plane.
I'd connect it to the RF GND at just one point, or better have both
faradayed before that.

Care has to be taken where the current returns. EG when you have a RC
on a digital line, the spike that disappears on the signal after the RC
is being lead to the GND at the C. And it propagates from there.
So GND is not GND but may have some mV of whatever on it.
This leads to differential signalling of sensitive signals, where also
the power supply rejection of the used components has to be taken into
account. Since all the spice simulation packages treat GND as GND,
they are useless in that aspect.

Another point : read the datasheets carefully.
Eg the analog GND and the digital GND of an ADC is to be connected
to the analog GND of the signal to measured only. The digital GND
is nowhere. The common mode rejection of the digital part allows
that.

Rene
 
Top