[SI-LIST] Re: Diff.Pairs

  • From: MikonCons@xxxxxxx
  • To: bmgman@xxxxxxxxxx, scott@xxxxxxxxxxxxx
  • Date: Mon, 13 Oct 2003 17:48:04 EDT

Scott & Mike:
You guys definitely have the right idea(s). One thing you forgot to mention, 
or that others on this thread might not have thought of, is that a reference 
plane between the traces of a "differential" pair provides excellent 
decoupling/isolation of signals on the two traces. In addition to the 
variations in 
effective dielectric constant (and its negative impacts on skew and even-mode 
impedance), the plane provides electrical isolation between the top and bottom 
surface plane currents via the skin effect. Even a 1/2-ounce copper plane would 
provide 26 dB reduction in magnitude of the image plane return current from one 
side of the plane to the other at only 120 MHz. The isolation is virtually 
complete for the GHz data rates that this thread addresses. I echo Scott's 
disdain for any high-speed design for differential pairs to use this approach.

RE: Scott's comment below,

"For vias spaced larger than 150 mils away from a ground via (most signal 
vias), there is about -0.8 dB insertion loss at 3 GHz.  This is 
comparable to a an 8.8% reduction in the signal amplitude of a 100 ps 
edge.  At 7 GHz (50 ps rise time) there is a -1.5 dB loss (16% amplitude 
reduction.)  These may or may not be significant losses in a design, but 
are extremely significant to the noise and EMI profile of a board, since 
all of this energy is being injected into the planes where it is not 
well contained.  The implication for 2.5, 3.125 and 10 Gbps PCB designs 
is profound.  Decouple the differential vias and get ready for increased 
losses, increased noise and increased EMI."

I couldn't agree more. As supporting evidence over the last four years, I was 
the third (and only successful) consultant to analyze and define routing 
rules for multi-GHz boards and backplanes for Nokia Networking. I found it 
necessary to use closely-coupled, coplanar pairs in open field routing, and 
symmetrical traces within pin fields that bracketed other differential pairs 
(to obtain canceling common-mode coupling fromn each +/- pair bracketed). My 
first guidance was to NOT use vias if at all possible. For unavoidable 
conditions, I devised a via structure that widened the narrowly spaced pair 
traces and 
bracketed two ground vias before coming back to close spacing on the new 
coplanar routing layer. The structure created a vertical two (round) wire pair 
100 Ohms differential impedance for minimal signal disturbance at the layer 
transition. Other consultants had tried multiple loosely-coupled techniques for 
1.5 years without acceptable results (names withheld as they are too 
recognizeable). In other words, tight coupling was the only viable solution, 
along with 
carefully designed via-pair transitions.

Keep up the good comments for the less experienced designers out there! Good 
thoughts also for Wyland and Knighten contributions.

It's 70 degrees, sunny, and the trout are rising. Bye.


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:

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

List archives are viewable at:     
or at our remote archives:
Old (prior to June 6, 2001) list archives are viewable at:

Other related posts: