Cortland Richmond <[email protected]> wrote:
> Current flowing through a via or a capacitor creates a voltage drop
>which drives the planes it connects, as a radiator. A good antenna
>may be made out of planes connected by a via, with RF applied
>between them. We need to avoid doing this by _accident_!
Assuming we are referring to small SMD components. The voltage drop across
a capacitor, (in this instance I take it that you meant the bypass
capacitor) is a function of the gap between the vias from the power and
ground planes. Here is another little trick, but it is subjected to having
the manufacturing and assembly people cooperating on this issue of board
performance.
I must caution that this stage of development in general, manufacturing do
not allow placing a pair of closely spaced via (pwr & gnd) right under a
cap. In ASCII art the plan view of the pad and via combo looks like this.
[]:[]
This however would push the typical resonance by a few octave over the
conventional layout and it is dependent on the thickness of the board.
The next step in the development is to boast the ability of the buried
capacitance by inserting a 0603(1.6x0.8x0.8 mm) sized capacitor vertically
into a hole on the PCB and solder the top and bottom ends. This have been
found to fit well in the standard 1.6 mm thick board. The hole can have
partial plate through.
Again in ASCII art the elevation view looks something like this.
] C [
A ===== pwr and ground layer
] P [
I can not wait to drive all the PCB shopfloor and assembly people up the
wall every time I come up with an innovation.
cheers
Tim Foo
Cortland Richmond
<72146.373@compuserve. To: John Coyle
<[email protected]>, ieee pstc list <[email protected]>
com> cc: (bcc: Wan Juang
Foo/ece/staff/npnet)
Sent by: Subject: Re: EMC & SIX
LAYER PCB
owner-emc-pstc@majordo
mo.ieee.org
04/04/02 01:35 AM
Please respond to
Cortland Richmond
A good thread. Some additional thoughts. This is a favorite question of
interviewers hiring EMC engineers (any reading?): "How would you stack this
board?"
Looking at the problem as controlling impedance, things fall into place.
Impedance to signal returns is impedance to signals. One SHOULD avoid
switching reference planes. But the effect of switching reference planes is
reduced if the potential required to pass return current between them -
impedance, including between sides of the SAME plane - is minimized, which
is where nearby "ground" via's and bypass capacitors come in.
Current flowing through a via or a capacitor creates a voltage drop which
drives the planes it connects, as a radiator. A good antenna may be made
out of planes connected by a via, with RF applied between them. We need to
avoid doing this by _accident_!
The return path for a trace penetrating a reference layer should be as
close as possible to the penetrating signal. While having it further off
does not change the via's impedance, it does require current flowing
through it to go further and increases the size of the radiating and
coupling loop. This is also an impedance inserted in series with the
desired signal.
A bypass capacitor is is not only a path for return currents, but a place
where cross talk can occur; it is a common impedance for all currents which
flow through it, and voltage across it is in series with signals whose
currents pass through it. If it is used to pass signal return currents, it
needs to be sized not only for the current demand of devices its storage
supplies, but also for the edge rate of signals whose return currents pass
through it. If it is operated above self-resonance, it _may_ form a
parallel resonant circuit with parasitic capacitance (or other capacitors),
and add unexpected impedance to the signal return. At the right (wrong)
place this can do a good impersonation of the feed to a patch antenna.
It is common now to use a pair of planes, power and ground, sometimes on a
very thin layer (AKA "buried capacitance") to minimize power supply
impedance. Unless this pair is rather extensive, it will need to be
augmented by discrete bypass capacitors, which should not have long via's
connecting them. This means near the surface. Signal traces need to be near
planes for high-frequency return currents. BGA technology requires
micro-via's between devices and surface or deeper planes. In addition,
building boards, we seem to prefer pretty much constant trace width and
spacing even while controlling impedance, and this means interior traces
need to be further away from planes for the same impedance at a given
width.
(Differential traces really should be coupled much more to each other than
to nearby planes, though often this is ignored. Providentially, yesterday's
mailbox brought the IEEE Transactions on Electromagnetic Compatibility,
volume 44, which includes on page 11 an analysis of what I've been yelling
at engineers for years. Heh! See:
_The Impact of a Nonideal Return Path on Differential Signal Integrity_,
Per Fornberg, Mark Kanda, Christopher Lasek, Melinda Piket-May and Stephan
H. Hall.)
Adding all the above, I come up with something like
1. TRACE R : route slower nets and break out BGA's
THIN : lower impedance of surface traces
2. POWER : return paths for upper layer
THIN : semi-"buried capacitance"
3. GROUND : Bulk caps are on top.
NORMAL : raise impedance to next trace layer
4. TRACE : high speed, between planes
NORMAL : raise impedance to adjacent traces
5. GROUND : return for high frequency currents on adjacent and surface
layer
THIN : lower impedance for surface layer
6. TRACE : surface layer
This does somewhat violate copper symmetry about the core, and may cause
complaints from the fab shop. It CAN be done. It will also cause headaches
in routing on a dense board, as it allows only three dedicated trace
layers. Portions of the ground and power planes may be used for routing.
They will be anyway, right? Just control impedance and coupling.
The issue of which goes next to the surface, ground or power, is an open
one. Consider impedance when you decide. Some people like ground layers on
the surface. REALLY high speed boards may need this. But it gives the
board fab shops screaming fits and hurts yield. At only 66 Mhz, you should
not have to need to do that.
Cheers,
Cortland
-------------------------------------------
This message is from the IEEE EMC Society Product Safety
Technical Committee emc-pstc discussion list.
Visit our web site at: http://www.ewh.ieee.org/soc/emcs/pstc/
To cancel your subscription, send mail to:
[email protected]
with the single line:
unsubscribe emc-pstc
For help, send mail to the list administrators:
Ron Pickard: [email protected]
Dave Heald: [email protected]
For policy questions, send mail to:
Richard Nute: [email protected]
Jim Bacher: [email protected]
All emc-pstc postings are archived and searchable on the web at:
http://ieeepstc.mindcruiser.com/
Click on "browse" and then "emc-pstc mailing list"
-------------------------------------------
This message is from the IEEE EMC Society Product Safety
Technical Committee emc-pstc discussion list.
Visit our web site at: http://www.ewh.ieee.org/soc/emcs/pstc/
To cancel your subscription, send mail to:
[email protected]
with the single line:
unsubscribe emc-pstc
For help, send mail to the list administrators:
Ron Pickard: [email protected]
Dave Heald: [email protected]
For policy questions, send mail to:
Richard Nute: [email protected]
Jim Bacher: [email protected]
All emc-pstc postings are archived and searchable on the web at:
http://ieeepstc.mindcruiser.com/
Click on "browse" and then "emc-pstc mailing list"
