Re[4]: impedance across ground plane

Tomm V Aldridge ([email protected])
Fri, 23 Feb 96 16:38:00 PST

Text item:

I agree with Ed's conclusions from a systems point of view but what happens
internal to a multi layer high speed board always leaves me with a slightly
unclean feeling.

Consider a board stackup that has signals referenced against both ground and
power planes. from an AC point of view the power planes are as good as ground.
If the signal is driven in reference to that plane (usually not the case) it
will work fine. If the signal is ground referenced, and uses the power plane
for impedance control, it will work fine if the plane is decoupled to the
driver's reference electrically close to the driver and to the receiver. Now,
if the signal is routed via vias in a dense board to use multiple power and
ground planes as its reference, how do I assure or even model signal integrity?

One suggestion is that at each via, a matching ground to voltage plane
decoupling cap be added. Any ideas?

______________________________ Reply Separator _________________________________
Subject: Re: Re[2]: impedance across ground plane
Author: [email protected] at SMTPGATE
Date: 2/23/96 5:01 PM


In the design of high performance digital circuits, read that as maintaining
specified edge rates for clock rates >40 -50 MHz, the concept of earth
ground never comes into the equation. The gentleman from the University of
Missouri, Prof Hubing, is exactly correct, namely that currents return to
their source. This is just another way of saying that the sum of the
voltages around a loop is zero and the sum of currents at a node is also
zero. Energy returns either by direct conduction, ie. currents or through a
coupling field.

The concept of earth ground vs. logic return ground is of course confusing.
In some equipment, especially in the European telephony area, chassis ground
and logic ground MUST be isolated. In the computer industry, the golden
"single point" ground has been the EMI model. Both these items are SAFETY
related issues and have nothing to do with EMI compliance or for that matter
impedance across a high performance PCB.

However, both these are necessary to be taken into account if one wants to
sell equipment on the world market. Specific solutions to the radiated EMI
problem says that common mode voltages between the logic and chassis ground
must be engineered to be as small as possible to meet the defined standard.
One can achieve this by either tying logic ground to chassis ground by a low
impedance connection. The single point ground meets this criteria, at least
at low frequencies (small in the Length/lamda) sense. When the frequencies
in question are higher and the signal spectrum is wider, then multi-point
grounding becomes more popular. But its just the need to maintain connection
densities that are small in the Length/lamda sense or equivalently small in
the Area/lambda**2 for loops. This approach sort of guarantees that even if
the system radiates, it does not do it well and the fields are evanescant
(non-propagating) around the equipment.

The alternative is to maintain no connection ie., current = 0 between the
chassis (earth) ground and the logic ground. This is much harder to achieve
since high frequency fields radiate and parasitically couple, particularily
to cabling leaving the enclosed Faraday shield which one invariably
constructs out of the chassis metal to contain the fields from the logic
cards. This is a tough approach to enforce.

What then is the story for signal integrity and EMI? One must keep the
currents and logic fields confined to the logic cards. Recognize that power
supply cables don't carry high frequency switching currents, so provide
local energy storage in the form of bulk and properly spec'd high frequency
bypass capacitors. Do not perforate the power and ground planes so
thoroughly that the ASIC's and high density connector effectively cut the
planes into sections. EMI and signal integrity problems come from such
constructions. Check the finished artwork to see that the CAM process
doesn't result in the same type of bisected planes condition. The board
fabrication process wants bigger anti-pads than might be good for signal
integrity and EMI system health.

| ------------------------------------- |
| "High Performance Engineering & Design" |
| Dr. Ed Sayre e-mail: [email protected] |
| NESA, Inc. |
| 636 Great Road Tel +1.508.897-8787 |
| Stow, MA 01775 USA Fax +1.508.897-5359 |

Text item: External Message Header

The following mail header is for administrative use
and may be ignored unless there are problems.


Cc: [email protected]
Subject: Re: Re[2]: impedance across ground plane
From: "Dr. Edward P. Sayre" <[email protected]>
To: [email protected] (Barry Ma)
Content-Type: text/plain; charset="us-ascii"
Mime-Version: 1.0
X-Mailer: Windows Eudora Light Version 1.5.2
X-Sender: [email protected]
Received: from by via smap (V1.3)
id sma003537; Fri Feb 23 17:01:11 1996
Message-Id: <[email protected]>
Date: Fri, 23 Feb 1996 17:01:41 -0500
Received: by mercury.Sun.COM (Sun.COM)
id OAA11798; Fri, 23 Feb 1996 14:03:49 -0800
Received: from mercury.Sun.COM (mercury.EBay.Sun.COM) by Eng.Sun.COM (5.x/SMI-5.
id AA24629; Fri, 23 Feb 1996 14:04:06 -0800
Errors-To: [email protected]
Received: from Eng.Sun.COM (engmail1) by silab.Eng.Sun.COM (4.1/SMI-4.1)
id AA02113; Fri, 23 Feb 96 14:04:31 PST
Errors-To: [email protected]
Received: from silab.Eng.Sun.COM (silab-188.Eng.Sun.COM) by Eng.Sun.COM (5.x/SMI
id AA10123; Fri, 23 Feb 1996 14:05:07 -0800
Received: by mercury.Sun.COM (Sun.COM)
id OAA12279; Fri, 23 Feb 1996 14:05:13 -0800
Received: from mercury.Sun.COM by (8.7.1/10.0i); Fri, 23 Feb 19
96 14:25:13 -0800
Received: from by (8.7.1/jIII); Fri, 23 Feb 19
96 14:25:25 -0800 (PST)
Received: from by with smtp
(Smail3.1.29.1 #4) id m0tq5vb-000HzAC; Fri, 23 Feb 96 14:25 PST