From: Mary ([email protected])
Date: Mon Nov 13 2000 - 09:46:53 PST
I attended a presentation by Prof. Hubing a few years ago. This
is from my notes:
On boards with power and ground planes spaced 10 mils
or less, location of the decoupling capacitors is not
important. Connect directly to planes with lowest
possible inductance.
On boards with power and ground planes spaced 30 mils
or more, locate decoupling caps nearest the pin that
connects to the most distant plane. (e.g. on a 4-layer
board with power on layer 2 and ground on layer 3,
active devices on layer 1 should have a cap near their
ground pin but active devices on layer 4 should have the
cap near their power pin.) This is to take advantage
of the mutual inductance between vias between the planes.
On boards without planes, minimize the inductance of the
connection between power/ground pins and the decoupling
capacitor.
He referred to a paper describing the mutual inductance
phenomenon, but I don't have that reference.
Mary
-----Original Message-----
From: [email protected]
[mailto:[email protected]]On Behalf Of Thomas Jackson
Sent: Monday, November 13, 2000 9:43 AM
To: 'si-list'
Subject: RE: [SI-LIST] : deCoupling caps and there placement
I would like to call you attention to:
"Power Bus Decoupling on Multilayer Printed Circuit Boards" by Hubing,
Drewniak, Van Doren and Hockanson, published in the May 1995 IEEE
Transactions on Electromagnetic Compatibility, Vol. 37, No.2.
Among their conclusions is that "on printed circuit boards that do have
internal power and ground planes, all decoupling capacitors are shared in
the frequency range in which they are effective (typically below 200-300
MHz), and the location of a decoupling capacitor on the board is relatively
unimportant."
It appears to be more important to have the shortest possible connections
between the decoupling capacitors and the power and ground planes than where
they are on the board.
Thomas L. Jackson, P.E.
Staff Product Development Engineer
Network Access Development
Systems Solutions Group
FUJITSU MICROELECTRONICS, INC.
3545 North First Street
San Jose, CA 95134-1804
telephone: (408) 922-9574
facsimile: (408) 922-9618
http://www.fujitsumicro.com
-----Original Message-----
From: [email protected] [mailto:[email protected]]
Sent: Monday, November 13, 2000 6:41 AM
To: [email protected]; [email protected]
Subject: Re: [SI-LIST] : deCoupling caps and there placement
Keith,
My approach is to put bypass capacitors as close as possible to the power
pins
on a chip. Whether we are using a multilayer card with ground and power
planes,
or a double-sided card with ground gridding, we will almost always have more
connections to and more copper for ground than for any one supply voltage.
Thus
the path from a bypass capacitor to ground is usually shorter and wider than
the
path to a supply voltage. This results in:
* Faster response by the capacitor, due to shorter transit time in the
microstrip/stripline between the chip and the
capacitor(s)--about 1/6 ns per inch for FR-4 boards.
* More return-paths to the chip for the transient current, which reduces
the
inductance, impedance, L * dI/dt drop, and
maybe radiated emissions by the magnetic fields of the various paths
partially cancelling one another.
* Smaller loop area for the transient currents, ditto.
Since transient currents are my major concern, I try to put the highest
frequency-response capacitors (typically 220pF NPO ceramics for clock and
phase-locked loops (PLL's)) right next to their corresponding power pins.
Then
I put lower frequency-response capacitors (typically a 100nF X7R ceramic for
each power pin or cluster of power pins) as close as possible to their
corresponding power pins. Next I consider how to route traces/vias to bring
power and ground to the power-pin/ground-pin/bypass capacitor cluster. If I
can
I will bring in power and ground right next to each other, but I don't worry
too
much if the power and ground connections are on opposite sides of a cluster.
Depending on the complexity and package size of the chip, I will also put 1
to 4
bulk ceramic capacitors (typically 2.2uF Y5V ceramics) on each supply
voltage
within 1 inch of its power pins, trying to "surround" the chip. If I have
a
bunch of small chips in a small area, I may use just one bulk ceramic
capacitor
for the entire clump.
Finally I put bulk aluminum electrolytic or tantalum capacitors (10uF and
up):
* Near the power connector(s) to a card.
* Near power connectors to other cards/devices.
* Near the corners of the supply-voltage domain.
* Near "power hog" components, trying to have one within 2 inches of every
power pin on that supply voltage ("coffee
cup" rule).
John Barnes Advisory
Engineer
Lexmark International
**** To unsubscribe from si-list or si-list-digest: send e-mail to
[email protected]. In the BODY of message put: UNSUBSCRIBE
si-list or UNSUBSCRIBE si-list-digest, for more help, put HELP.
si-list archives are accessible at http://www.qsl.net/wb6tpu
****
**** To unsubscribe from si-list or si-list-digest: send e-mail to
[email protected]. In the BODY of message put: UNSUBSCRIBE
si-list or UNSUBSCRIBE si-list-digest, for more help, put HELP.
si-list archives are accessible at http://www.qsl.net/wb6tpu
****
**** To unsubscribe from si-list or si-list-digest: send e-mail to
[email protected]. In the BODY of message put: UNSUBSCRIBE
si-list or UNSUBSCRIBE si-list-digest, for more help, put HELP.
si-list archives are accessible at http://www.qsl.net/wb6tpu
****
This archive was generated by hypermail 2b29 : Tue May 08 2001 - 14:30:05 PDT