[SI-LIST] Re: Copper Fill
- From: MikonCons@xxxxxxx
- To: si-list@xxxxxxxxxxxxx
- Date: Fri, 14 Jun 2002 14:53:54 EDT
A stimulating thread I can no longer resist commenting on.
Thermal distribution is aided by more copper (pointed out by at least two
others).
Additional copper thieving by the board fabricator to achieve more even
copper throw should be comprised of small patches of copper (more on this
later) and adhere to the approximate spacing guideline of 3 x Dielectric
thickness (noted by Lee Ritchey) away from traces on the same layer AND on
adjacent layers (for the same rationale; i.e., impedance loading). I've noted
>10% loading caused by this effect. Small copper patches (for thieving) do
not need to be individually grounded as their fundamental resonance will be
in the high GHz region, which is above the frequencies of interest for most
of today's boards.
However, I soundly disagree with some comments in this thread about fills NOT
being a potential EMI issue, and about grounding of fills. First, with the
edge rates achieved by current semiconductor technologies, any surface
conductor over 1/4 inch should be used with care. Current induced in surface
fills through electromagnetic coupling WILL cause radiated emissions to
occur. Its only a matter of antenna efficiency (a strong function of
frequency/harmonics/edge speed) of the fill as to whether it becomes of
concern or not.
Inadvertent antenna formation can occur with slots in planes (slot antenna)
and copper patches. These structures are routinely used in microwave antenna
designs, particularly for flat, antenna arrays and for the "skins" of
missiles. Slots and patches are used also as impedance matching elements to
achieve maximum power transfer to surface antennas. There was a special issue
of the Proceedings of the IEEE dedicated to this topic in January 1992. Check
it out for a good overview of the 30 or so different antenna structures and
an excellent article (with illustrative pictures) of the coupling structures.
Scott's comments on grounding fills and adding what I call "spoiler" vias to
form a gridded connection to the internal ground plane(s) is right on target
at avoiding efficient "antennas" and minimizing radiated emissions. These
grounded patches of fill serve as field termination points for emissions
generated by traces and package structures on the board surface. We all know
that high frequency signals will take the path of least impedance to return
to their reference. The grounded fills provide the most convenient
termination path to fields that are generated above the board assembly by
signal currents in the vicinity of the fills. The net effect is to reduce the
radiated emissions that WOULD occur without the grounded fills. Note: Similar
field termination effects are achieved by chassis-grounded guard rings around
the periphery of boards.
Grounded fills also help lower the overall impedance of the board ground
structure which has a very positive effect in suppressing common-mode voltage
development. This in turn will minimize radiated emissions from any cables
connected to the board assembly.
In my designs, I take advantage of any open areas on the surface layers of
boards to a) add shielding and field termination surfaces, b) parallel ground
(or power) planes with fills (connected by the noted vias) to lower the board
common mode impedance, c) lower the board thermal conductivity to minimize
temperature and localized physical stresses, and d) increase board stiffness
for less flexure over life. Using these (and other) techniques on problem
boards I have been called in to "fix," I have routinely achieved a 15 to 25
dB reduction in radiated emission levels for more than 20 clients and over
100 different boards in the last 10 years.
The following comment by Alex McPheeters is right on target. "Though this is
far off the original topic, we all should know and your selection of
bare-board vendor should also know that they should never 'assume' anything,
today's PCB's tolerate very little assuming..."
Mike
Michael L. Conn
Owner/Principal Consultant
Mikon Consulting
Cell: (408)821-9843
*** Serving Your Needs with Technical Excellence ***
------------------------------------------------------------------
To unsubscribe from si-list:
si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field
or to administer your membership from a web page, go to:
//www.freelists.org/webpage/si-list
For help:
si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field
List archives are viewable at:
//www.freelists.org/archives/si-list
or at our remote archives:
http://groups.yahoo.com/group/si-list/messages
Old (prior to June 6, 2001) list archives are viewable at:
http://www.qsl.net/wb6tpu
Other related posts:
