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