Re: [SI-LIST] : Slightly different signal integrity problem

Pat Zabinski ([email protected])
Wed, 13 Jan 1999 09:02:12 -0600


There are several possible explanations for what you are experiencing,
and it's very difficult to nail down the real reason without
much more info/tests. However, here's a few things I've
noticed in the past that might be helpful. When you do resolve/fix
the problem, please let us all know, as this is a common problem
in mixed-signal designs.

In terms of shielding, you definitely want to ground the shield
to the ground plane. In fact, you want the shield to make electrical
contact with the plane around the entire periphery; do not leave
any large gaps in the connection between the plane and shield. Openings
in the shield often act like openings in waveguide, which is
pseudo-equivalent to a waveguide horn antenna. At a bare minimum,
make sure no gaps exist larger than 1/4 wavelength of the highest
frequency of interest (I generally try to achieve <1/10 wavelength,
but this is not always possible).

In the worst case, if the shield is ground at just a single point,
the shield will act like a monopole (mono-mess?) antenna, in which
case you'll be picking up gobs of stray EM.

When you mention the "circuit can be made to trigger by touching the ground
plane with a metallic object", it makes be believe that the problem might
be due to ground loops. If you have any loops in the ground connections
between the board, the test equipment, power supply, etc., stray
magnetic fields can induce currents, which in turn can cause problems
similar to what you're experiencing. The tried-and-true method to
avoid this is to arrange all ground contacts such that there is only
one common point with no possible loops. Generally, arranging the
grounds in a "star" pattern with the common node at the DUT works

If the problem is with stray EM, one way to get around this is to completely
change your power supply connections to the DUT. Two-layer boards are
great when the boards are small enough to avoid resonance, but this
is not always the case. In cases where the board is larger than
1/2 wavelength of the highest frequency, it quite often helps to
keep the solid ground plane (with shield directly attached per above)
and replace the power plane with traces. The traces will increase
the inductance, which will in turn increase the EM noise rejection
to the device. You need to be concerned, however, that switching
noise on the DUT will also be increased (as many SI folks will tell
you), so this technique is not always applicable (best in current-
steering vs current-switching technologies).

One last possibility is resonance in your decoupling scheme. If your
board has several capacitors for decoupling the supplies, it
is quite possible that the decoupling capacitors are either resonating
with the trace/pin inductance (in the case of a single supply level)
and/or the supplies are oscillating between themselves through
the capacitors (in the case of multiple supply levels). In either
case, adding series resistance (2-6 ohms will generally do the
trick) to the decoupling will damping the resonance/oscillations.

Let me (us) know what finally works,
Pat Zabinski

On Jan 12, 3:38pm, Lund, Steve wrote:
> Subject: [SI-LIST] : Slightly different signal integrity problem
> Dear SI-list Members,
> I have a question regarding a slightly different signal integrity problem.
> Please forgive me if this is considered off-topic.
> I have an application that receives optical pulses through plastic optical
> fiber and directly into an infrared receiver IC for conversion back into an
> electrical signal. The IC in question is an LTC1328. This chip is intended
> for the standard IRDA protocols which has a certain amount of error
> rejection built-in. In my application the pulses are used as received and
> there is no optical "noise" due to transmission over a plastic fiber.
> The problem that we have noticed is stray pulses being received as a result
> of stray EM fields. We have decided to mount the receiver IC on a double
> sided PC board (about 3/4" square) with ground plane on the solder side and
> a metal shield on the top side. However, there is still one open issue. In
> the current configuration without the shielding on a double sided board with
> ground plane there appears to be noise also picked up due to disturbances on
> the ground plane. The circuit can be made to trigger by touching the ground
> plane with a metallic object such as a screwdriver or connecting a scope
> probe ground even when connecting at the opposite corner of the current 2" x
> 3" PC board.
> Because of this I am seeking your input as to the advisibility of a
> separating the signal ground from the shield on the receiver module. The
> receiver IC in an SO-8 package has a single pin for both analog and digital
> ground and this same pin is also one of the photodiode inputs which may be
> the path for the ground induced noise.
> So I guess the question is this: Should the shield be isolated from circuit
> ground and if so how? Thanks for any and all suggestions.
> Steve Lund
> Tuthill Transfer Systems
> **** To unsubscribe from si-list: send e-mail to [email protected]
In the BODY of message put: UNSUBSCRIBE si-list, for more help, put HELP.
si-list archives are accessible at ****
>-- End of excerpt from Lund, Steve

**** To unsubscribe from si-list: send e-mail to [email protected] In the BODY of message put: UNSUBSCRIBE si-list, for more help, put HELP. si-list archives are accessible at ****