I agree that interplane capacitance between closely spaced planes is very
valuable as high-frequency decoupling, but I would add a caution to relying
on it for continuty of the return path. It will work or not depending on the
application, the size of the board and the frequencies of the return
currents that needs continuity.
In the case of a 100mmX100mm board with 8 mil spacing between a PWR and a
GND plane, I calculate the parasitic capacitance to be about 2nF. That
represents an impedance of about 0.8Ohm which would be OK for many
applications (but not all). At 1MHz the impedance is 80Ohm, and in most
applications this will force the return current to flow places you don't
want it. It will work poorly for much of the noise generated by switching
power supplies, as an example. Smaller layer spacing improves the situation,
smaller boards makes it worse. The designer must in any case calculate the
capacitance and assure himself/herself that it is adequate in each case, not
rely on it as a general rule.
I would also keep in mind that the interplane capacitance is distributed.
For very large return currents this will cause the current to flow
throughout the planes with potential differences across the planes as
possible results. It is better to use a single net for all AC return as far
as possible. And this is not even thouching on the problems that arise when
power planes with multiple power domaines are used as return
The comment about not using discreet capacitors for return at frequencise
higher than a few hundred MHz is very good. It is very risky to not have an
explicit return i copper for high-frequency buses. Any use of capacitive
return must be made with close attention to the inductance in the
connection, also interplane capacitance.
Med vennlig hilsen/Best regards
________________________________________________
Haldor Husby, Senior Development Engineer
Data Respons Norge AS
Kongsberg Næringspark
P.O. Box 1022
N-3601 Kongsberg, Norway
Tel: +47 32 29 94 00 Fax: +47 32 29 94 40
Dir: +47 32 29 94 18 Mob: +47 48 04 83 68
[log in to unmask]
On Thu, 4 Jan 2007 12:35:59 -0600, Susy Webb <[log in to unmask]> wrote:
>Hi Jack....
>
>The ideal choice is to reference the signal to opposite sides of the same
plane when it must change directions, but that cannot alwyas be done.
Another option as you said, is to reference two different ground planes
because the return can move very easily through the vias.
>
>But returning signals on power layers will work too. You should ALWAYS have
power and ground layers next to each other at least once in your stackup for
medium to high speed boards. If the power and ground are close to each other
<.008" then the signal return can couple from one plane to the other and
back to the source.
>
>As an example, if you consider the source of the energy to be the cap near
an IC, the energy then flows from the power side of the cap to the power pin
of the part, then through the part and out the signal pin and out onto a
signal layer. Let's say that signal layer references the ground plane, and
that ground plane is part of a plane pair. When the signal has to change
direction, it moves to the signal layer on the other side of the plane pair
and the return now references the power plane. The return on the power plane
can capacitively couple to the ground plane because they are so close to
each other and then find it's return path back to the source... the ground
side of the cap. This does not increase the inductive loop because the
return path does not have to separate from the original signal. Remember,
returnis happening constantly, not just at the end of the signal.
>
>If the power and gound planes are separated, this will not work and you
will be relying on capacitors for return as you mentioned. HOWEVER, the
faster the frequency, the more limited the usage of the capacitors (even
high frequency ones), and they are virtually useless above 2-300 MHz. So it
is better to use the inter-plane capacitance of having the two planes together.
>
>Hope this is clear enough to understand.... it's hard to describe in text
what a picture would easily draw.
>Susy
>
>>
>> From: Jack Olson <[log in to unmask]>
>> Date: 2007/01/04 Thu AM 09:50:41 CST
>> To: [log in to unmask]
>> Subject: [DC] Straddling the Return Path
>>
>> I have a question about layer stackup and routing.
>>
>> Most of our designs have a pair of routing layers
>> sandwiched between planes, one for vertical and
>> the other for horizontal traces.
>> Maybe I haven't had enough coffee yet today, but
>> I started wondering how the return path energy
>> gets from one plane to the other (unless there
>> happens to be a decoupling cap nearby?) If both
>> planes were GND there wouldn't be a problem,
>> since they would be stitched together in many
>> places, but one is GND and the other is PWR.
>>
>> So I started wondering.... Wouldn't it be better to
>> have one routing layer ABOVE the GND plane and
>> one BENEATH? In this scheme all the routing would
>> be straddling the SAME return path and it seems
>> logical the it would be less noisy. There would never
>> be a discontiuity from the energy trying to get from
>> one plane to the other, right?
>>
>> maybe the gains are not worth the loss in the
>> overall scheme, though?
>>
>> onward thru the fog,
>> Jack
>>
>>
---------------------------------------------------------------------------------
>> DesignerCouncil Mail List provided as a free service by IPC using
LISTSERV 1.8d
>> To unsubscribe, send a message to [log in to unmask] with following text in
>> the BODY (NOT the subject field): SIGNOFF DesignerCouncil.
>> To temporarily stop/(restart) delivery of DesignerCouncil send: SET
DesignerCouncil NOMAIL/(MAIL)
>> Search previous postings at: www.ipc.org > On-Line Resources & Databases
> E-mail Archives
>> Please visit IPC web site
http://www.ipc.org/contentpage.asp?Pageid=4.3.16 for additional information,
or contact Keach Sasamori at [log in to unmask] or 847-615-7100 ext.2815
>>
---------------------------------------------------------------------------------
>>
>
>---------------------------------------------------------------------------------
>DesignerCouncil Mail List provided as a free service by IPC using LISTSERV 1.8d
>To unsubscribe, send a message to [log in to unmask] with following text in
>the BODY (NOT the subject field): SIGNOFF DesignerCouncil.
>To temporarily stop/(restart) delivery of DesignerCouncil send: SET
DesignerCouncil NOMAIL/(MAIL)
>Search previous postings at: www.ipc.org > On-Line Resources & Databases >
E-mail Archives
>Please visit IPC web site http://www.ipc.org/contentpage.asp?Pageid=4.3.16
for additional information, or contact Keach Sasamori at [log in to unmask] or
847-615-7100 ext.2815
>---------------------------------------------------------------------------------
---------------------------------------------------------------------------------
DesignerCouncil Mail List provided as a free service by IPC using LISTSERV 1.8d
To unsubscribe, send a message to [log in to unmask] with following text in
the BODY (NOT the subject field): SIGNOFF DesignerCouncil.
To temporarily stop/(restart) delivery of DesignerCouncil send: SET DesignerCouncil NOMAIL/(MAIL)
Search previous postings at: www.ipc.org > On-Line Resources & Databases > E-mail Archives
Please visit IPC web site http://www.ipc.org/contentpage.asp?Pageid=4.3.16 for additional information, or contact Keach Sasamori at [log in to unmask] or 847-615-7100 ext.2815
---------------------------------------------------------------------------------
|
