Henry Ott Consultants

Electromagnetic Compatibility Consulting and Training

Grounding of Mixed Signal PCBs

A question that I hear often is:  How do I prevent digital logic ground
currents from contaminating my low level analog circuitry?  This is a good
question without a simple answer.  Most A/D converter manufacturer's data
books and application notes provide little if any useful information on the
subject.  If they do provide information, it is usually only applicable to
a simple system containing only one A/D converter.

Some people suggest splitting the ground plane in order to isolate the
digital ground currents from the analog ground currents.  Although the
split plane approach can be made to work, it has many potential problems
especially in large complicated systems.  Can you list some of these
problems?  One of the major ones is that you can not route a trace over
the split in the plane (see Tech Tip Slots in Ground
Planes).  It is always better to have only a single reference
plane for a system.

If you do split the ground plane and run traces across the split (left hand
figure below), there will be no return path near the trace and the current will
have to flow in a big loop.  Current flowing in big loops produce
radiation and high ground  inductance.    If you must split
the ground plane and run traces across the split,  you should do it as
shown in the right hand figure below.  By connecting the planes together
at one point (a bridge) and routing all the traces so that they cross at this
bridge point, you will have provided a return path for the current directly underneath
each of the traces (hence a very small loop area).

High
frequency digital ground return currents want to return directly underneath the
signal trace.  This is the lowest impedance (lowest inductance)
path.  The digital ground currents have no desire to flow through the
analog portion of the ground plane and corrupt your analog signal.  Why
then do we need to split the ground to prevent the digital current from doing
something that it does not want to do anyhow?  Therefore, I prefer the
approach of using only one ground plane and partitioning the PCB
into digital and analog routing sections.  Analog signals can then
be routed only in the analog section of the board (on any layer), and digital
signals can  be routed only in the digital section of the board (on any
layer).  What causes problems is when a digital signal is routed in the
analog section of the board, or visa versa.

A PCB with a single ground plane, partitioned into
analog and digital sections, and discipline in routing
the signals can usually solve an otherwise difficult layout problem, without
creating the additional problems caused by  a split ground plane.  If
the layout is done properly, the digital ground currents will remain in the
digital section of the board and will not interfere with the analog
signals.  The routing, however, must be checked carefully to assure that
the above mentioned routing restrictions are adhered to one hundred
percent!   The key to a successful mixed signal PCB layout,
therefore, is proper partitioning and routing discipline, not a
split ground plane.

Many A/D converter manufacturers, while suggesting the use of split ground
planes, state the following in their data sheets or application notes:
"The AGND and DGND pins must be connected together externally to the same
low impedance ground plane with minimum lead length.  Any extra external
impedance in the DGND connection will couple more digital noise into the analog
circuit through the stray capacitance internal to the IC."  Their
recommendation is to connect both the AGND and the DGND pins of the A/D
converter to the analog ground plane.  This approach has the potential of
creating a number of additional problems.  Can you list some of these
problems?  What do you connect the ground side of the digital power
decoupling capacitor to?  The analog plane or the digital plane?

A much better way to satisfy the requirement of connecting AGND and DGND
pins together through a low impedance, and not create additional problems in
the process, is to use only one ground plane to begin with.

The key to determining the optimum board layout is to think, how and
where do the return currents flow?

If you are still skeptical about using a single ground plane on your mixed
signal boards I suggest you do the following experiment.  Layout the board
with a split ground plane, but provide means for connecting the two planes
together every 1/2 inch with jumpers or zero ohm resistors.  Route the
board properly, with no digital traces (on any layer) over the analog plane and
no analog traces (on any layer) over the digital plane. Build the board and
test it's  functionality and EMC performance.  Connect the planes
together and test the board again for functionality and EMC performance.
I think that you will find that in almost all cases, both the functional
performance and the EMC performance of the board will be better with the single
ground plane.  If you do the experiment  send me an e-mail letting me
know of your results.

It is almost always better to have only a
single reference plane for a system!

Analog ground plane noise voltages should be kept smaller than the
minimum  analog signal level of concern.  In the case of an A/D (or
D/A) converter the smallest resolvable signal voltage level [least significant
bit (LSB)] is a function of the number of the bits and the full scale reference
voltage of the A/D converter. The smaller the reference voltage and the larger
the number of bits, the smaller the minimum resolvable signal voltage will be.
The following table shows the resolution versus the number of bits for an A/D
converter using a one volt reference.  These resolution levels can be
scaled for other reference voltages by multiplying the resolution by the
appropriate factor.  For example, if the converter uses a 5 volt reference
then multiply the resolution numbers in the table by five.

Number of Bits

Resolution (LSB)

8

4 mV

10

1 mV

12

240 uV

14

60 uV

16

15 uV

20

1 uV

24

0.06 uV (60 nV)

The
use of a single solid ground plane  properly partitioned and routed (as
discussed above) is usually adequate for most low to moderate resolution A/D
converters (8, 10, or 12 bit).  For higher resolution systems (14 bits and
up) even more ground noise voltage isolation may be required for adequate
performance.  These converters have resolution voltages in the tens of
microvolts, or less, level.  In this case you might want to divide your
board into separate isolated analog and digital ground plane regions, each
solidly connected to the digital ground plane under each of the A/D converters
as shown in the figure. This approach will provide additional ground noise
isolation for the high resolution A/D converters while still maintaining a
single ground plane for the system.

Notice that even in this case, the ground plane is not split --  it is
all connected together.  Also remember that no traces, on any layer, can
cross over the isolating slots in the ground plane.

Summary

Partition your
PCB with separate analog and digital sections.

Do not split
the ground plane.  Use one solid ground plane under both analog and
digital sections of the board.

Route digital signals only in
the digital section of the board.  This applies to all layers.

Route analog signals only in
the analog section of the board.  This applies to all layers.

The key to a successful PCB
layout is the use of routing discipline.

© 2000/2003 Henry W.
Ott
Henry Ott Consultants,  48 Baker Road  Livingston,  NJ
07039  (973) 992-1793

Bibliography

Ott, H. W., Partitioning
and Layout of a Mixed Signal PCB, Printed Circuit Design, June
2001.

Correspondence

Thank you, this article will
assist me in a proposal I made earlier this week in a design review on how
to properly layout and partition a PCB with analog and digital
signals.  As you can probably imagine I was met with major opposition
when I proposed utilizing a bridge to connect the analog and digital
sections.  I have used this technique on other PCB's (different
Business Unit) and had no problems although I never had the opportunity to
conduct the experiment and analyze the data as you mention in your
article, thank you very much. [e-mail from an engineer in Michigan]

I am in the process of laying
out a mixed-signal board myself and your article has provided some useful
information.  Thinking of the issue in terms of return current flow makes
a lot of sense. [e-mail from a RF Engineer in California]

Your tech tip "Grounding
of Mixed Signal PCBs" was the most clear and concise presentation of
the material that I found.  Everyone else suggest separate planes
connected at a single point but neglect to consider "big loops"
as you suggest. Since you so clearly articulated (i.e., helped me
understand the real issue), I am planning on purchasing your book to hopefully
better understand EMC design issues. [e-mail from an engineer in Arizona]

I am busy designing a mixed
signal board incorporating two 16-bit DACs and a high-speed digital side,
and found your website very enlightening.  It's amazing how much info
there is out there by supposed "experts" that is clearly
outdated or not very well thought through, and your website provided a
welcome change.  [e-mail from a post-graduate student in South
Africa]

Return to top of page.

Return to HOC home
page.

Henry Ott Consultants

48 Baker Road Livingston, NJ 07039

Phone: 973-992-1793,   FAX: 973-533-1442

March 25, 2004