[SI-LIST] Re: Buried Capacitance thread comments (The whole t hing)
- From: MikonCons@xxxxxxx
- To: si-list@xxxxxxxxxxxxx
- Date: Tue, 4 Dec 2001 17:07:21 EST
In a message dated 12/3/2001 2:40:58 PM Pacific Standard Time, from
chris.cheng@xxxxxxxxxxxx:
[Chris] Sometimes it is lumped into the so called SSO (ground/
power bounce) noise problem. I hope we agreed that this is an issue
related to I/O switching current return path.
[MLC] The EMI/radiated emissions deal with both. I understand you have placed
the emphasis on the latter.
[Chris] In my opinion (and here is where I think the
agreement starts to diverge) the return path management happen
either on die through on die decoupling (actually we still agree
on this) or manage the signal reference planes.
[MLC] We are in substantial agreement here, but I would change the "...or
manage..." to "...and manage..."
[Chris] Here lies the
problem with 2 mil power/ground planes, they cannot be used for
the signal reference planes since the impedance control of the
signals dictated the thickness of the dielectric. In order to
used this 2 mil core dielectric, your signal traces have to be
super thin, something the current PCB technology is not possible
to achieve.
[MLC] This may be where we appear to disagree, but I think it is actually a
misunderstanding. I would never try to put the signal traces between the
layers of a 2-mil BC sandwich as it is indeed impossible to fab such narrow
traces. Both surfaces of the BC sandwich can be used as reference planes;
i.e., signal traces can be placed on either side of the sandwich. The very
low ac impedance between the two planes (I'm referring to >50 MHz region)
allows drivers and receivers using the same power and ground associated with
the BC sandwich to operate efficiently (i.e., with small mode conversion).
[Chris] Like I said in previous messages, if microstrip signal
traces on the package or on the PCB happens to be referencing to
the wrong power planes (a very very common mistake designers
made, in particular on low cost low layer count PCB), you will
see the resonance/EMI/SSO noise you mentioned.
[MLC] This is indeed a common mistake by many designers. However, the
resulting radiated emissions caused do not need to excite a board resonance
to cause regulatory limits to be exceeded. The errant current return path is
akin to building in a loop antenna on the PCB whose efficiency goes up as
frequency squared. As you note, the board dimensional resonances can be
excited and will worsen the problem.
[Chris] But the problem can also be eliminated simply by bring the signal
to at least one proper reference plane (typically ground plane)
and provide an even lower impedance return path than 2mil planes
or lots of decoupling caps.
[MLC] For signal excitation, we are in absolute agreement. However, if the
planar noise is caused by SSO effects on the chip power/ground interface(s),
board resonances will be excited. Then, the BC approach is your (next?) best
friend because of its basic low impedance and lossy characteristic at higher
frequencies.
**********
Note that poor high frequency signal path design can destroy EMI performance,
as is emphasized by Chris. Additionally though, the excitation of planar
resonances can come from multiple sources including poor signal return paths,
power supply and/or ground bounce from SSO in multiple chips (not just
processors), impulse (i.e., leading edge) noise from switching power
supplies, etc. The locations of the different offenders/exciters on the board
is also a factor as the PCB will behave as a patch antenna. This is where
edge stitching (which can raise the resonance by a factor of two) and
grounded outboard guard traces (which act as field interceptors), as well as
other techniques, come into need. Each potential noise excitation source
needs to be considered by the board designer to achieve a "minimal emission"
design.
Good engineering to all.
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:
