[SI-LIST] Re: Buried Capacitance thread comments (The whole thing)

Scott old pal, this is neither a fight, non am I Irish.
You make some good reference on the imperfect nature of image
current return. Lets take a closer look.
 
As performance increases, people use different techniques to
address this issue. In the not so distant past, open drain (like GTL) or
emitter follower (like PECL or ECL) I/Os are used and they are by
design asymmetric I/O that only need a single reference plane for
current return to the driver (the other direction is being taken
cared by the decoupling at the terminator) In the case of GTL, all
the return path needs to reference is ground (Bill Gunning used
to joke with me saying "don't call this Gunning transceiver logic, call
it ground transceiver logic).  Similar argument for PECL or ECL
I/O's. 
In lots of new high speed designs differential signals are use in
which they reference to themselves (in differential mode) and 
asymmetrical reference to the terminating voltage (common mode).
 
From the above, asymmetric I/O is more popular than you think, 
but we still have to address the push pull drivers. It turns out in 
order to sustain the sharp edge rate even to come out of the 
package, a lot of those I/O uses on die decoupling to support 
the initial di/dt. As such they can (while "not desire" as you 
like to say) take return current asymmetrically, either from the
ground or the i/o power through the on die decoupling.
Most likely they will take the ground path for the return.
As you mentioned, a lot of packages have to use microstrip
to route the signals out. However, the so call mode conversion
will happen at the die level through the on die decoupling such
that once it comes out of the die, only ground reference is
need for both transition image current to return. In that
situation, either case 1) or 3) in your description will
be just fine for the I/O. You can even project to case 2)
is ok provided the power plane is the I/O power and the
package reference planes is either power or sandwich
between power and ground.
 
What you didn't mention is what I consider case 2b) 
where the reference power plane is not even the I/O
power e.g. the other power plane at a different level.
In this situation, your mode conversion or image
current return is broken. This is where people see
EMI noise or signal power/ground bounce. This is
when people bring in those EMI or SI consultants
where they start to sprinkle in those 100's of
pf decoupling caps or Zycon planes to provide
the low impedance path for the image current to
return. In my opinion, two wrongs doesn't equal 
to one right. The problem should be solved by properly 
referencing the signal return power/ground planes.
 
There is another case 1b) which the power plane 
in the power/ground stripline is not the I/O power 
but other power. In this case the image current 
in the power plane has to return through the plane
capacitance between the power/ground planes.
Unfortunately, the spacing of the planes are 
dictated by the impedance control of the striplines
and thin dielectric is just out of the question.

Finally, since you know me a little bit, you 
should know that I used to have the luxury of 6
well trained engineers doing power analysis
for me on package resonance. All the plane
resonance, via location, decoupling, plane
discontinuity analysis are BTDT. And guess
what, the package resonance hardly goes 
above 100MHz and you better believe I
have the best possible package design
available. Any other references you came
across are in the range of 10-40MHz. 
I have mentioned this fact many, many
times in this group and those who have
done the same analysis have to agree with
me. Am I trying to say PCB plane don't
resonance? Absolutely not. Does resonance
matter above 100MHz ? Probably not. 
 
I don't quote papers, I don't just say "you
are way off" without any reasons. I say what I
say because I've BTDT.
 
 -----Original Message-----
From: Scott McMorrow [mailto:scott@xxxxxxxxxxxxxxxx]
Sent: Thursday, November 29, 2001 1:02 AM
To: chris.cheng@xxxxxxxxxxxx
Cc: 'MikonCons@xxxxxxx'; si-list@xxxxxxxxxxxxx
Subject: Re: [SI-LIST] Re: Buried Capacitance thread comments (The whole
thing)



As the Irishman said: 

"Is this a private fight, or can anyone join?" 
  


Chris Cheng wrote: 


There are those who use scare tactics to justify their consulting 
jobs and academic life and there are those who have to do real 
designs and ship products.

Yes, and I believe Mike has a track record of many successful 
designs and products shipped over many years. 

What the paper didn't say is if you bury the signal trace with 
the proper reference planes and there by providing the lowest 
and tightest coupling return path, the EMI and noise will drop 
to beyond any 100's of caps or Zycon plane can provide you.

This is only correct if the same was done on the device at the 
package. (i.e. the signal is launched from the die onto stripline 
sandwiched between symmetric I/O power and ground planes, 
or proper return path structures.)  Unfortunately, most devices 
are not packaged in such a way.  The signal launch is generally 
referenced primarily to one plane or the other. 

In the case of an asymmetric launch, a mode has already been 
established between the signaling conductor and one or more 
reference conductors.  The best a board designer can do at 
this point is to maintain the same return path mode on transition 
from the package to the board.  In this way, mode conversion will 
not occur, or be minimized.  It is mode conversion that launches 
energy into the power and ground plates at the transition from the 
package to the board. 


Chris, you assume a purely symmetric return path at the die launch. 
This is not usually the case, unless specifically designed that way. 
I do agree that this would be the ideal, however impractical it might 
be for most designs, due to the added cost of multiple layer buildup
packages. 
For  the highest performance designs one must try to keep the signal 
return path continuous from package to board.  It is key to remember 
that the signal return path is not necessarily the same as the power 
return path.  In a perfect world, both would be the same.  Once the 
signal has been launched on a waveguide structure, and the fields 
have "adjusted" themselves to this condition, the wave does not care 
what potential the underlying guiding structure is at (power, ground or 
even floating.) 


It is the transition that is important, nothing more.  For a 
single ended I/O signal, the first transition which occurs is at the 
die/substrate boundary.  If the transition is asymmetric, as it often 
is, then some of the energy mode converts to the proper stripline or 
microstrip mode onto the substrate trace, and the remainder of  the 
energy mode converts to one of many power distribution modes (which 
depend on the package and die design.)  It is this first mode conversion 
at the die where a substantial amount of "power" noise is developed, and 
is due to imperfect substrate design.  Much of system noise has it's 
origins here. 


The next mode conversion that occurs will be in the necessary via 
transitions on the substrate as the signal winds it's way down to the 
ball layer.  Mode conversions here will launch energy from the via 
stack into the power and ground plate modes (assuming that power 
and ground planes actually exist in a particular package).  This, again, 
is totally dependent upon the design of the substrate and ball out 
pattern.  The ball (and via) pattern in the region of a particular 
signal escape should attempt to maintain a continuous return path 
from the substrate through to the board.  (i.e. if the substrate signal 
is mostly referenced to ground, then the neighboring vias and balls 
should be referenced to ground.  If the signal is mostly referenced to 
a particular power plane, then the neighboring vias and balls should 
be referenced to that same power rail. 


(The above can be quite easily verifed using full wave FDTD or 
frequency domain solvers.) 


If a designer has detailed knowledge regarding the package routing 
and signaling reference for each signal, then an optimal PCB (or MCM) 
routing solution can be generated that maintains the same launch 
reference across the Package/Ball/Board interface.  ( For example, if the
signal is 
referenced to ground, then it should be referenced to ground at the 
board to reduce mode conversion, noise and EMI.) 


Since most mortal designers do not have access to detailed knowledge 
regarding the package routing and signaling reference for each signal, 
a compromise solution is possible.  What you talk about (incessantly) 
Chris, is really just that, a "rule of thumb" compromise solution that 
works well in all systems.  That is, to route all PCB signals as stripline 
between an I/O power plane and a ground plane.  In fact, what I believe 
you advocate is this structure. 


-------------------- ground 
-------------------- power 
       ----          signal 
-------------------- ground 
-------------------- power 


This is the best possible compromise PCB signal routing geometry, when 
the designer does not have enough information to actually engineer the 
correct structure, due to limitations in the packages or knowledge thereof. 
It is, however, quite inefficient in terms of z-axis space utilization.  And
the 
method falls apart if a designer cares to utilize dual asymmetric stripline 
layers to reduce overall layer count and cost. 


For any signal that is launched from a package to a board, with a power and 
a ground plane, there are three possible basic signal/power waveguide 
modalities that can occur.  1) the signal is stripline and is between a
power and 
a ground plane.  2) the signal is microstrip or stripline and is referenced
to 
only a power plane.  3) the signal is a microstrip or stripline and is
referenced 
to only a ground plane.  (Actually, there are several others which we will
neglect 
for this discussion.) 


Now, assuming that the package waveguide modality was maintained through 
the the package vias and ballout, the "Chris Chang" method of signal routing

is optimal for only case number 1, where the signal is referenced to a power
and 
a ground plane.  Here this mode can be continued from the package through 
to the board without mode conversion occuring.  For cases 2 and 3, Chris' 
method is not optimal.  For example, a power plane referenced signal will 
need to mode convert at the transition to properly attach to the ground
plane 
of the PCB waveguide structure.  For case 2, the perfect PCB structure would

be power referenced microstrip or stripline (between two power planes). For
case 3, 
the perfect PCB structure would be ground referenced stripline or
microstrip. 


For cases 2 and 3, the mode conversion is handled by local power/ground
plane 
pairs on either side of the stripline.  This high quality distributed low
impedance 
LC circuit quickly provides closure of the return path, facilitating minimal
distruption 
during conversion to the proper stripline mode.  Noise is created on the
power 
and ground planes when the mode conversion occurs.  This noise will never 
be less than the optimal structure which maintains the same mode across the 
entire board from package to package. 


Sprinkle in hundreds of decoupling 
capacitors with different values and in different location. 
Then put in thousands of power and ground vias mimicking 
real life package power and ground pins. Stitch ground 
vias around the edge of the board like what real world 
design. Lets see if you still have your resonance. 
 

Absolutely.  All parallel plate waveguides resonate.  It is just a matter 
of the interactions of all the structures involved (planes, vias, splits, 
devices.)  In fact, all non perfectly terminated structures have multiple 
resonant eigenmodes.  Some which can have a quite high Q.  It's fairly 
easy to find the resonant modes with a VNA, a spectrum analyzer, or 
with some effort with full wave board simulation software.  With some of 
the new fast solver technology, we should start seeing some commercial 
solutions become available in the next few years.  In that case, we will 
all be able to simulate these sorts of full board problems in minutes
instead of 
hours or days. 
  

regards, 


scott 
  


-- 
Scott McMorrow 
Principal Engineer 
SiQual, Signal Quality Engineering 
18735 SW Boones Ferry Road 
Tualatin, OR  97062-3090 
(503) 885-1231 
http://www.siqual.com <http://www.siqual.com>  
  
  



-----Original Message----- 
From: MikonCons@xxxxxxx [ mailto:MikonCons@xxxxxxx
<mailto:MikonCons@xxxxxxx> ] 
Sent: Wednesday, November 28, 2001 6:38 PM 
To: si-list@xxxxxxxxxxxxx 
Subject: [SI-LIST] Buried Capacitance thread comments (The whole thing) 

[MLC] Sorry, Chris, but you are WAY off on this one. Check out the 
literature 
from 1989-1991 and the electronic "Product of the Year" award given to Zycon



for the ZBC 2000 product (the original name) for EMI reduction. I know you 
are practicing some good design to achieve Class B certification, but good 
power/ground plane decoupling plays a major part in that success. Many 
papers 
demonstrated attenuatin of 20-30 dB over all frequencies above 40 MHz when 
using BC and DELETING over 100 0.1 Uf decoupling capacitors. (Check with Dr.



Jim Howard at Sanmina, Santa Clara, CA if you doubt this.) Lee Ritchey 
commented correctly on the contribution of the planar decoupling. 
********* 
[MLC] Chris makes a key point in identifying the return path for any 
high-speed currents. However, the reference to the Zycon planes seems to be 
a 
slam at the benefits of that technology. If one studies RF techniques in 
depth, then the fact that for a given resonance frequency the Q of that 
resonance 
is decreased with increased capacitance. This is the unheralded forte of the



buried capacitance concept. I have performed spectrum analyzer tests (with a



tracking generator) on circular and square PCBs (11" diameter/side) 
employing 
BC that clearly demonstrated (relative to identical PCBs without BC) NO 
RESONANCE effects at high frequencies (>40 MHz). The effect of this 
characteristic is LOWER EMI that is (many times) caused by PCB dimensional 
resonances. This benefit is particularly useful for High-Tg FR-4 boards and 
higher frequency designs (>500 MHz) as the FR-4 losses play a significant 
role at the higher harmonics. 
********* 
>From the above comnments, I wish only to convey that we are all still 
learning, and an open mind is critical to solving the design challenges of 
the future. 


Mike 


Michael L. Conn 
Owner/Principal Consultant 


Mikon Consulting 


                   *** 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: 
http://www.freelists.org/webpage/si-list
<http://www.freelists.org/webpage/si-list>  


For help: 
si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field 


List archives are viewable at: 
                http://www.freelists.org/archives/si-list
<http://www.freelists.org/archives/si-list>  
or at our remote archives: 
                http://groups.yahoo.com/group/si-list/messages
<http://groups.yahoo.com/group/si-list/messages>  
Old (prior to June 6, 2001) list archives are viewable at: 
                http://www.qsl.net/wb6tpu <http://www.qsl.net/wb6tpu>  


------------------------------------------------------------------ 
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: 
http://www.freelists.org/webpage/si-list
<http://www.freelists.org/webpage/si-list>  


For help: 
si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field 


List archives are viewable at: 
                http://www.freelists.org/archives/si-list
<http://www.freelists.org/archives/si-list>  
or at our remote archives: 
                http://groups.yahoo.com/group/si-list/messages
<http://groups.yahoo.com/group/si-list/messages>  
Old (prior to June 6, 2001) list archives are viewable at: 
                http://www.qsl.net/wb6tpu <http://www.qsl.net/wb6tpu>  
 


  



------------------------------------------------------------------
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:
http://www.freelists.org/webpage/si-list

For help:
si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field

List archives are viewable at:     
                http://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: