# RE: [SI-LIST] : Upper limit of interplane capacitance

From: Larry Smith ([email protected])
Date: Tue Jun 13 2000 - 09:44:36 PDT

Larry - thanks for your comments.

Discrete decoupling capacitors run out of gas at about 500 MHz. We
have managed to reduce the mounting inductance for 0603 size capacitors
to 300 pH. If we assume 200 pH for the internal capacitance of the
capacitors, we have a total of 500 pH which is 942 mOhms at 500 MHz.
Discrete capacitors are not doing much good.

You can use the series resonant frequency and low ESR capacitors to
drive towards a low impedance at 500 MHz. But using the formula f0 =
1/(2pi*sqrt(LC)), the capacitance required to hit 500 MHz with 500 pH
ESL is about 200 pF. We get 225 pF for every square inch of power
planes (4 mil dielectric, FR4), so unless we are going to use more than
one discrete capacitor every square inch, they will not be of much use.

A far better solution is to get the low impedance from the power
planes. Using FR4 BC technology from Hadco (2 mils) we get 450 pF per
square inch. Dupont, 3M and other materials vendors are beginning to
advertise 1 mil dielectric cores that are compatible with PCB
manufacture. That brings us up to 900 pF per square inch. We are
beginning to get away from straight FR4 technology, but this is where
our industry needs to go if low impedance power distribution is
required at high frequency. If this thin dielectric has some high K
material in it, so much the better.

But almost more importantly, the thin dielectric material has low
spreading inductance. High capacitance and low inductance results in
lower impedance power planes and that is very good. There is no point
in putting a bunch of low impedance decoupling capacitors on a PCB if
you don't have low impedance power planes to hook them up.

The skin effect losses (alpha of a transmission line) go as
Rskin/2*Z0. Istvan Novak (Sun) has demonstrated how low impedance
power planes naturally damp out the cavity resonances because of skin
effect losses as the dielectric thickness drops to a fraction of a mil.
At more than 1 GHz, dielectric loss also contributes to the damping.
In this case, loss is a good thing.

So, the solution to low impedance power distribution above several
hundred MHz lies in thin dielectric power plane technology. This is
much more effective than discrete decoupling capacitors. (But Discretes
are not going to go away because they will be required at frequencies
below several hundred MHz.) With the attenuation from thin dielectric
power planes, the size of the planes (6x6 inches) becomes of minor
importance. I would not advocate carving up power planes, that only
leads to other problems.

regards,
Larry Smith
Sun Microsystems

> From: "Larry Miller" <[email protected]>
> Subject: RE: [SI-LIST] : Upper limit of interplane capacitance
> Date: Mon, 12 Jun 2000 11:08:29 -0700
>
> An excellent treatment.
>
> Taking all of this into account, what would you say is a rough limit
> frequency for PCBs and coupling caps as a circuit packaging methodology? It
> seems like it would be size dependent. For a 6 inch square effective board,
> maybe 1 GHz? Do you think you can extend this up by putting in stitched
> moats to subdivide a board into smaller effective sheets? Hoo-ha?
>
> Larry Miller
>
> > -----Original Message-----
> > From: Larry Smith [SMTP:[email protected]]
> > Sent: Monday, June 12, 2000 10:45 AM
> > To: [email protected]; [email protected]
> > Cc: [email protected]
> > Subject: Re: [SI-LIST] : Upper limit of interplane capacitance
> >
> > We have experimental data on power plane resonances and good model to
> > hardware correlation. There has been a lot of discussion of these
> > topics on si-list recently and I feel that it is time to comment.
> > Everyone in the industry is using power planes for power distribution,
> > but there does not seem to be good agreement for the behavior of these
> > planes or how to model and measure them.
> >
> > Take for example a pair of 1 oz copper planes separated by 4 mils of
> > FR4 with dimensions of 6 inches on a side. The planes behave like a
> > parallel plate capacitance at low frequency. The capacitance is
> > epsilon*area/thickness and works out to be 225 pF/square_inch or 8.1 nF
> > for the plane pair.
> >
> > The time of flight down the length of the planes is 1 nSec for e0=4
> > (FR4). A full wave will stand in the cavity at 1 GHz and a half wave
> > at 500 MHz and create high impedance resonances. From a point source,
> > the planes behave like a radial transmission line, but in my view, this
> > not very important. If a point anywhere on the board (except dead
> > center) begins to stimulate the planes at a multiple of 500 MHz (half
> > wavelength), energy builds up in the resonant cavity. After several
> > cycles, there are plane waves bouncing back and forth between the open
> > circuit ends of the planes. High voltage is always found at the edges
> > and high current nodes are found in the center of the planes. It doesn't
> > matter where the source is because the resonance is a function of the
> > cavity dimensions. All that is important is that the cavity got
> > stimulated.
> >
> > These effects can be measured nicely with a network analyzer. Connect
> > port 1 and port 2 just about anywhere on the board. It is best to
> > leave at least an inch between them so that the vertical connections do
> > not couple with each other. Fifty Ohm transmission line soldered to
> > empty decoupling capacitor pads work nicely for this. At low
> > frequency, the network analyzer will show you an impedance that
> > decreases with frequency at 20 dB per decade. If you do the math on
> > the impedance you calculate the plane capacitance, Z=1/(j*omega*C). At
> > frequencies below cavity resonance, all points on the power planes are
> > at the same potential at any given point in time and it does not matter
> > where the probes are located. For the 6x6 square inch example, this is
> > true up to about 100 MHz (1/4 wavelength stands in the board at 250
> > MHz).
> >
> > There are many ways to model this, but my favorite is a matrix of
> > transmission lines. We divide the board into an 8x8 array of 64
> > sections. Transmission lines are used to connect the nodes in an x-y
> > fashion. The transmission line parameters are easily calculated from
> > plane capacitance, inductance and resistance. Ray Anderson mentioned
> > some of these calculations last week. The calculations have been
> > documented by the HP guys at EPEP conferences and Journal articles over
> > the past couple of years. HSpice will allow .ac analysis on frequency
> > dependent resistors which are used for skin and dielectric loss.
> > HSpice also enables parameter calculations and it is possible to
> > calculate dB = 20*Log(V/I) to simulate the impedance that matches the
> > output of the Network analyzer.
> >
> > We have very good model to hardware correlation on bare fabs (unstuffed
> > PCB's) that correctly shows the capacitance at low frequencies and all
> > important cavity resonances up to several GHz. For cavity resonances,
> > the position of the probes on the power planes is very important to get
> > the low impedance dips associated with 1/4 lambda to a board edge. The
> > high impedance peaks occur at the same frequency everywhere on the
> > board but the magnitude of the peak varies with position. The height
> > of the peaks and depth of the valleys are determined by the Q of the
> > circuit which is a strong function of skin and dielectric loss at
> > cavity resonant frequencies.
> >
> > But all that changes as soon as decoupling capacitors and components
> > are mounted on the power planes. With well chosen decoupling
> > components, it is possible to make the impedance vs frequency flat up
> > to 100 MHz. The capacitors force he impedance of the planes to -60 or
> > -70dB from 30 kHz to 100 MHz where the bare fab was much higher than
> > that, perhaps -30 dB with a slope associated with 8.1 nF. Decoupling
> > capacitors still dominate the cavity resonances between 100 and 400
> > MHz, but the position on the power planes now becomes important.
> > Decoupling capacitor placement is important at these frequencies.
> >
> > One very important impedance peak occurs between the decoupling
> > capacitors (that have gone inductive) and the relatively pure
> > capacitance of the power planes. These two elements form a parallel LC
> > tank circuit with a high impedance resonance, usually at several
> > hundred MHz. If the discrete capacitors are well distributed on the
> > power planes (as they usually are on our products), we have an
> > inductance and capacitance per square area and position on the PCB is
> > not important. This impedance peak must be carefully managed,
> > particularly if we have taken advantage of low ESR capacitors to
> > minimize the number of mounted components. It is usually more of
> > an EMI problem than an SI problem.
> >
> > We notice several dB of change above 100 MHz when a large uP is
> > inserted or removed from it's socket. It takes a lot of careful
> > modeling of the active devices and the decoupling capacitors mounted on
> > pads and vias to get the simulated models to match the hardware
> > measurements. (but that is beyond the scope of this already long
> > email..).
> >
> > regards,
> > Larry Smith
> > Sun Microsystems
> >
> > > Date: Fri, 09 Jun 2000 14:44:30 -0700
> > > From: "Douglas C. Smith" <[email protected]>
> > >
> > > I am not a guru on this topic either, however I have thought
> > > that there is more than a radial transmission line here, in
> > > that the two dimensional transmission line has lots of funny
> > > mid-plane loads in the form of bypass capacitors that give
> > > reflectons (I am talking of power to ground plane here).
> > > That combined with the open sides would make for a driving
> > > point impedance that would should be quite lumpy with
> > > frequency. I am ignoring the lossy loads of the devices
> > > themselves which are another set of complicating factors.
> > >
> > > Does anyone have experimental data they have taken on this
> > > handy?
> > >
> > > Doug (Smith)
> > >
> > > Doug McKean wrote:
> > > >
> > > > "Chan, Michael" wrote:
> > > > >
> > > > > I would like to point out that what would be the impedance look like
> > when
> > > > > you looks at it from the center of the two plates viewing from the
> > top? Can
> > > > > you still qualify it as a rectangular wave guide as the wave is
> > spread out
> > > > > in
> > > > > 360 degree other than in one particular direction. Instead of
> > calling it the
> > > > >
> > > > > traditional "characteristic impedance" I would prefer to see it as "
> > driving
> > > > >
> > > > > point impedance". Any comment from any guru ????
> > > >
> > > > The "equations" come out the same. Just as if you
> > > > were asking if there would be any difference with
> > > > the characteristic impedance of a one dimensional
> > > > transmission line at the end or in the center.
> > > > Reality would dictate something different with the
> > > > geometries and cutouts in the planes.
> > > >
> > > > But there's a couple of different issues going on
> > > > with parallel plates structures and quite different
> > > > in many ways. One structure is that the parallel
> > > > plates make a transmission line, the other is that
> > > > they make a waveguide. The transmission line supports
> > > > electric and magnetic fields in the dielectric as
> > > > currents move in the plates. The waveguide simply
> > > > *guides* fields between them. either along the axis
> > > > of the plates or by reflecting them off the walls.
> > > >
> > > > In the case of the plates constituting a transmission
> > > > line, circulating currents say in the power plane would
> > > > terminate at the edges. Since there's no termination
> > > > at the edge, this would cause theoretically a complete
> > > > positive reflection.
> > > >
> > > > Like ripples on a pond, these would create nodes at
> > > > various points about the planes depending upon many
> > > > factors geometry being one. Which is in fact the case.
> > > > Termination of such could not be accomplished with
> > > > a single point connection such as a resistor.
> > > >
> > > > This phenomena cannot be explained when considering
> > > > the planes as a *waveguide*.
> > > >
> > > > - Doug McKean
> > > >
> > > > **** 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
> > > > ****
> > >
> > > --
> > > -----------------------------------------------------------
> > > ___ _ Doug Smith
> > > \ / ) P.O. Box 1457
> > > ========= Los Gatos, CA 95031-1457
> > > _ / \ / \ _ TEL/FAX: 408-356-4186/358-3799
> > > / /\ \ ] / /\ \ Mobile: 408-858-4528
> > > | q-----( ) | o | Email: [email protected]
> > > \ _ / ] \ _ / Website: http://www.dsmith.org
> > > -----------------------------------------------------------
> > >
> > > **** 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 : Wed Nov 22 2000 - 10:50:36 PST