|
Ground Impedance and Interconnect
By William D. Kimmel, P.E.
and Daryl D. Gerke, P.E.
We find that an overwhelming number of EMI problems have
ground impedance at the root. Oftentimes the problem is not
obvious until you take a close look. The problems are often
at the circuit board and at the interconnect. Let’s take
a look at the basic issue and where it can occur.
Ground Impedance
Figure 1 shows the basic issue – a driver and receiver
with associated return (ground) path. The ground impedance
creates a potential problem both for emissions and immunity.
For emissions, the voltage drop across the return path creates
a common mode voltage. As shown, this forms a dipole antenna
– not an efficient antenna, but adequate to cause emission
problems, even if the return path is unbroken copper. But,
as we shall see, the actual case may be much worse.
The reciprocal case occurs with immunity. In Figure 1 an ESD
pulse bounces the ground, causing an error signal to appear
between driver and receiver.
Note that if the ground impedance is zero, there is no problem.
In the real world we can’t get to zero, but there are
certainly things we can do to effectively reduce the impedance.
First thing to note is that impedance of a ground plane is
much less than that of a trace (as would be found on a two-layer
circuit board). In round numbers, at 100MHz the impedance
of even a short (one cm) trace is in the neighborhood of 10
ohms, whereas the impedance of two points on a plane is about
10 milliohms. That’s a factor of one thousand times.
How much difference does this make? Let’s consider an
ESD pulse injected into a ground pin of a circuit board. One
amp of ESD current will bounce the ground of a one cm trace
approximately 10 volts, more than enough to cause a data error.
The same pulse will bounce a ground plane only 10mV. Yet,
an ESD pulse can be 10 amp or more. Clearly, we have a problem.
That is why we say that you must keep ESD off a two-layer
board at all costs – you will not recover. But even a
poorly designed multilayer board will create problems, as
we will see below.
We have a similar problem on the connector, where the ground
path is one or more pins each with length of a couple of centimeters
or more. On a cable, of course, the lengths are much longer.
How to Fix
When we start a design project, ground impedance is always
at the forefront of our thoughts. But the first order of business
is to identify the critical signals. For emissions, it is
almost always the periodic or near-periodic signals, usually
a clock line or switching power supply line, sometimes a data
bus. While emissions are pretty well confined to a few chips
and signal paths, immunity issues can occur at any signal
path – a single signal error, even on a low speed line,
can cause an irrecoverable error. But most immunity threats
enter from off the board at the periphery of the circuit board.
Having decided on the critical signals, we look to how to
keep the relevant ground impedances as low as possible, and
this includes maintaining return path continuity.
On the Circuit Board
How do we reduce the ground impedance on the circuit board?
Let’s start by looking at multilayer boards – we’ve
already discussed the low impedance of a ground plane. But
even there, lots of things can go wrong. Keep your eye on
the return path – if it is directly underneath the signal
trace along the entire path, then you have done a good job.
If there are any deviations, then you have room for improvement.
Figure 2 shows several examples where the return is discontinuous.
The first is simply a break in the ground plane – a slice
was taken out of the plane to make room for another trace:
bad news. The second is a plane change – the return path
is broken at the via – return currents have to divert
to the nearest decoupling capacitor. In principal, the return
path will be through the plane capacitance – in practice,
this path doesn’t become adequate until you are nudging
1Ghz.
The key is to keep the return path continuous. Don’t
run the trace across a slot in the plane. Avoid switching
planes, but if you must go through a via, drop a ground via
(in the case of a ground to ground return path) or a decap
(in the case of a ground to voltage return path).
If you are working with a two-layer board, your ground impedances
are always high, and you have to work very hard to get the
impedances down to a tolerable level, if you can do it at
all. Start by looking at the return path – make sure
it parallels the signal path, either underneath or alongside.
Keep the critical signal lines short. If possible, allocate
ground area underneath the signal path.
At the Connector
Inadequate number of ground pins in the connector is one
of the most common problems we encounter: What? Waste connector
pins on grounds?
Figure 3 shows the common situation – too many signal
pins sharing the few grounds allotted. Any transient currents
crossing the connector boundary will bounce the ground. Also
note that the poor placement of the signal pin/ground pins
creates a large loop area, degrading the signal and potentially
creating differential mode loop radiation.
Again, there is no substitute for a ground plane. For board-to-board
interconnect, a ground strap keeps the impedances low. For
a cable, a microstrip line is the answer.
Lacking a ground plane, you will need plenty of ground pins,
sprinkled throughout the connector, rather than bunched at
one end. Alternating signal and ground pins is the best combination
and, in demanding cases, mandatory. For less demanding cases,
you might get by with one ground per five signals, making
sure the critical signals are placed adjacent to a ground
pin. Anything less than one ground per five signals and you
are looking for trouble.
Summary
When working with EMI or ESD problems, always keep ground
impedance at the top of your requirements list. Remember to
maintain return path continuity – easy to do on cables,
but often neglected on circuit boards and connectors. Designs
that have inadequate grounding are hard to fix, often requiring
a major re-do.
|
