From: Larry Miller (email@example.com)
Date: Tue Aug 15 2000 - 09:33:33 PDT
I think Pat's points are well-taken.
Unless you are using ECL I think that you will find the situation
self-limiting. For example, with BGAs it is not unusual to have on the order
of 1 nH of inductance on the spreader board between the actual chip and the
PCB (which brings up other problems, but never mind....)
You certainly need to be thinking in terms of matched impedance PCB traces.
I have had very good luck considering 100 MHz-ish parts to have 10 to 30
ohms driving impedance (gotten from a least-squares fit to some IBIS data).
This seems to hold up retty well over a number of vendors and geometries in
the 0.25u range.
Since most PCBs are set up with 50 ohm traces these days, that says you need
source terminator resistors. This can also get out of hand, and I have had
good luck making the PCB traces lower impedance. Unconventional, but try it
with SPICE. You do end up with 10 to 15-mil wide traces, but in a tight
layout thsi is OK if you have lots of layers.
Bear in mind that if you end up with calculated values that won't fit you
have a situation where the chip vendors could not sell their wares! (See
Pat's example below)
My experience on this has been in the gigabit Ethernet area. (PHYs and MACs,
switch fabrics and SDRAMs)
I have found that if you
1) put a ring of 0603 caps outside a BGA ball pattern on the bottom side
2) put another ring inside (between the BGA ball pattern for signals and the
group of balls in the middle used for thermal grounding, if present), also
on the bottom side
3) use a 50-50 mix of values of .01 uF and .001 uF, and
4) add a few bulk tantalums near the corners of the BGA
you will be all right if
5) you have good ground and power planes in the center of the stackup with
close spacing (.005" or so) between them.
If it takes more than this, let's face it, you have a real problem....
> -----Original Message-----
> From: Zabinski, Patrick J. [SMTP:firstname.lastname@example.org]
> Sent: Tuesday, August 15, 2000 8:41 AM
> To: email@example.com
> Subject: RE: [SI-LIST] : Decoupling capacitors (again!)
> I can't offer much advice, but I can possibly offer some
> comfort in that I've had the same problem. For one design
> I was recently involved in, I tried to follow the same
> approach/theory, and the end result was that I needed
> 80 decoupling capacitors per ASIC (to maintain 10%
> dV), and I had 32 ASICs per board (>2500 caps per board!).
> After having others verify
> my numbers/calculations, I took close look and realized
> the caps would consume more board space than the ASICs.
> I could not justify, believe, or afford this, so I
> ended up backing down and relying on my old rules of
> thumb (BTW: I hate rules of thumb, but I sometimes
> use them when I have no better way). The board works
> fine with only 12 caps per ASIC.
> Looking back, I can see three possible reasons why the approach you
> and I took is not quite complete:
> * component packaging effects are not taken to
> account. Not definite on this, but I believe
> a poor package would probably negate any capacitance
> you might have on the board.
> * the board's self-impedance. I believe Larry's
> approach addresses this as effective increase
> in inductance, but the ground/power plane itself
> does offer a low-impedance capacitance. Regardless
> if you have any discrete caps on or not, the planes
> offer some inherent, built-in capacitance.
> * most (all?) dI/dt effects are self-limiting.
> For the calculations you used, they assumed
> dV=0.0. However, if dV>0, then dI/dt will
> be reduced all on its own. I don't have any
> data or theories on how much, but dI/dt
> is likely to be reduced from what you
> predicted (also tied into/related to the
> first issue about packaging).
> Sound reasonable? Comments?
> Anyway, I sympathize and hope you find a solution. If you
> do, please share.
> > -----Original Message-----
> > From: Martin J Thompson [mailto:Martin.J.Thompson@trw.com]
> > Sent: Tuesday, August 15, 2000 9:49 AM
> > To: <"firstname.lastname@example.org"
> > Subject: [SI-LIST] : Decoupling capacitors (again!)
> > Hi all, this is my first time posting here, although I've
> > been lurking for a while.
> > My problem is figuring out the decoupling requirements for
> > this system:
> > FPGA, DSP, 6 SDRAMS, 2 flash, DPRAM, clock frequency is 100MHz.
> > According to my calculations, my I/O's need to drive a total
> > of about 1.5nF of I/O and trace capacitance.
> > To achieve the 0.5ns edges that the FPGA will drive (3.3V
> > supply) it looks like I need dI=4amps. This is assuming that
> > 50% (is this typical?) of the I/O's toggle each cycle. (dI=0.5Cdv/dt)
> > To achieve a dV of < 0.1V this implies a target impedance of
> > around 20mohm, flat up to 1GHz! (Z=dv/di)
> > This then seems to need around 500-800 decouping caps spread
> > around, which is an order of magnitude more than I've ever
> > used in the past. This is the first time I have taken a
> > 'design' approach to the problem, but the previous boards
> > have worked, using various rules of thumb.
> > Is this sort of number of caps to be expected in this sort of
> > system, or can anyone see any sillies in my understanding (or
> > even in the sums!)?
> > Now, if I don't get right out to 1GHz, the edges will suffer,
> > but that wouldn't necessarily matter if they stayed below
> > 1-1.5ns. Or would this cause the supply to droop elsewhere?
> > As you might gather from the analysis above I've read Larry
> > Smith and co's paper on decoupling design, which states that
> > a flat target impedance is indicated. If I can analyse my
> > application enough, can I then shape the Ztarget vs frequency
> > to make life easier?
> > Many thanks for your time, any help greatly appreciated,
> > Martin
> > TRW Automotive Advanced Product Development,
> > Stratford Road, Solihull, B90 4GW. UK
> > Tel: +44 (0)121-627-3569
> > mailto:email@example.com
> > **** To unsubscribe from si-list or si-list-digest: send e-mail to
> > firstname.lastname@example.org. 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@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
**** To unsubscribe from si-list or si-list-digest: send e-mail to
firstname.lastname@example.org. 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 : Wed Nov 22 2000 - 10:51:02 PST