From: Doug Brooks (email@example.com)
Date: Mon Nov 13 2000 - 16:36:34 PST
I interpret it just as it says and as Todd says in the interview.
The study that said "the location of the decoupling ...unimportant" (which
study is referenced in footnote 4 and which study is the oft quoted Tod
Hubing, et al study of 1995) applied only to narrowly spaced planes (10
mils), and not to other configurations. Therefore, the "unqualified"
extension to the idea that placement in unimportant (in general) is
projecting beyond the validity of the study. The paper in 1995 simply does
not show that placement is unimportant in the general case --- only in the
case where the planes are closely spaced (within 10 mils.)
At 03:57 PM 11/13/00 -0700, you wrote:
>Mark & Doug,
>How do you interpret that?
>[mailto:firstname.lastname@example.org]On Behalf Of Mark Gill
>Sent: Monday, November 13, 2000 11:16 AM
>To: 'Doug Brooks'; Thomas Jackson; email@example.com
>Subject: RE: [SI-LIST] : deCoupling caps and there placement
>Folks - Just a note on the UMR work. To quote a UMR sponsored paper for
>the 2000 EMC symposium, "Quantifying Decoupling Capacitor Location", the
>"A more recently published study of decoupling capacitors and printed
>circuit boards as ensembles concluded that for printed circuit boards with
>both power and ground planes, all decoupling capacitors are shared in the
>frequency range in which they are effective; hence, the location of the
>decoupling capacitor on the board is unimportant . This study
>considered multi-layer boards with closely spaced layers and its
>conclusions may have been extended beyond the region of validity of the study."
> T. Hubing, J. Drewniak, T. Van Doren, and D. Hockanson, "Power Bus
>Decoupling on Multilayer Printed Circuit Boards," IEEE Transactions on
>Electromagnetic Compatibility, Vol. 37, No. 2, pp. 155-166, May 1995.
>Mark Gill, P.E.
>EMC/Safety/NEBS Design & Compliance
>C-MAC Engineering Design Services
>From: Doug Brooks [<mailto:firstname.lastname@example.org>mailto:email@example.com]
>Sent: Monday, November 13, 2000 12:23 PM
>To: Thomas Jackson; firstname.lastname@example.org
>Subject: RE: [SI-LIST] : deCoupling caps and there placement
>But, I too would call your attention to an article that appeared in PC
>Design Magazine in March, 1998 titled "An Interview With Todd Hubing" (a
>reprint is available in the "articles" section of our web site at
><http://www.ultracad.com>http://www.ultracad.com). Todd qualified the
>comments in the article you
>referenced as applying only to boards where the power planes were 10 mils
>or less apart. For more conventional structures he commented that "closer
>There has been a great deal of misinterpretation of what the results meant
>in Todd's earlier article, and the Interview was an attempt to help clarify
>some of the questions.
>At 07:42 AM 11/13/00 -0800, you wrote:
> >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
> >It appears to be more important to have the shortest possible connections
> >between the decoupling capacitors and the power and ground planes than
> >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
> >-----Original Message-----
> >From: email@example.com
> >Sent: Monday, November 13, 2000 6:41 AM
> >To: firstname.lastname@example.org; email@example.com
> >Subject: Re: [SI-LIST] : deCoupling caps and there placement
> >My approach is to put bypass capacitors as close as possible to the power
> >on a chip. Whether we are using a multilayer card with ground and power
> >or a double-sided card with ground gridding, we will almost always have
> >connections to and more copper for ground than for any one supply voltage.
> >the path from a bypass capacitor to ground is usually shorter and wider
> >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
> >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.
> >I put lower frequency-response capacitors (typically a 100nF X7R ceramic
> >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
> >power and ground to the power-pin/ground-pin/bypass capacitor
> cluster. If I
> >I will bring in power and ground right next to each other, but I don't
> >much if the power and ground connections are on opposite sides of a
> >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
> >within 1 inch of its power pins, trying to "surround" the chip. If I have
> >bunch of small chips in a small area, I may use just one bulk ceramic
> >for the entire clump.
> >Finally I put bulk aluminum electrolytic or tantalum capacitors (10uF and
> >* 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
> > Lexmark International
>Doug Brooks' book "Electrical Engineering for the Non-Degreed
>Engineer" is now available. See our web site for details.
>Doug Brooks, President firstname.lastname@example.org
>**** To unsubscribe from si-list or si-list-digest: send e-mail to
>email@example.com. In the BODY of message put: UNSUBSCRIBE
>si-list or UNSUBSCRIBE si-list-digest, for more help, put HELP.
>si-list archives are accessible
Doug Brooks' book "Electrical Engineering for the Non-Degreed
Engineer" is now available. See our web site for details.
Doug Brooks, President firstname.lastname@example.org
UltraCAD Design, Inc. http://www.ultracad.com
**** To unsubscribe from si-list or si-list-digest: send e-mail to
email@example.com. 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 - 14:30:07 PDT