Re: [SI-LIST] : Broadside Coupled Traces

Fred Balistreri (fred@apsimtech.com)
Thu, 22 Apr 1999 12:02:32 -0700

Ron Miller wrote:
>
> In theory broadside traces have the advantage of relying less on the
> ground for
> impedance and could work with no groundplane at all, so they could go
> across a
> pcb and various planes with impunity.
>
> In practice, since we are limited to about 3 or mils minimum trace
> widths by the
> board houses, the increased height for 50 ohms(100 ohms differential)
> starts to take up a lot of the thickness available in the board.
> Also, the increased height between ground
> planes makes cross coupling worse between pairs. In order to reduce
> the coupling
> between pairs on the same layer you should figure that spacing =3 X
> Height(ground to ground plane) will give about 40 db or .01 X voltage
> coupling at the worst frequency
> considered.
>
> With differential traces on the same layer this spacing is relatively
> easy to get. With
> broadside coupled lines you have 3 sandwiched layers of dielectric,
> and the top
> and bottom dielectric must be 2 or 3 times thicker. Then the spacing
> between pairs
> goes up as a factor of about 5.
>
> So, with broadside coupled lines you will get a reduction in density
> to about 1/10 of what
> you get with standard differential traces on the same layer.
>
> Ron Miller
>
> mannand@wlgore.com wrote:
>
> Can anyone outline the advantages and disadvantages of using
> broadside coupled
> vs. edge coupled differential traces? Is either one better
> from a signal
> integrity perspective ( less lossy? lower crosstalk?). Is
> it easier to route
> broadside coupled traces in high density applications? And
> what are the issues
> board manufactures need to deal with such as tolerances,
> trace registration,
> impedance control, number of layers, etc.? Any insight you
> can provide would be
> helpful. Thanks!
>
> **** To unsubscribe from si-list: send e-mail to
> majordomo@silab.eng.sun.com. In the BODY of message put:
> UNSUBSCRIBE si-list, for more help, put HELP. si-list
> archives are accessible at http://www.qsl.net/wb6tpu/si-list
> ****
>
> --
> Ronald B. Miller _\\|//_ Signal Integrity Engineer
> (408)487-8017 (' 0-0 ') fax(408)487-8017
> ==========0000-(_)0000===========
> Brocade Communications Systems, 1901 Guadalupe Parkway, San Jose, CA 95131
> rmiller@brocade.com, rbmiller@sjm.infi.net
>
>
Somebody is confused about differential signals. The whole idea of
having differential signaling involves tight coupling. If you
seperate the traces such that they are not coupled then they are not
differential signals. Now there are papers that conclude differential
impedance is not needed for digital signals running on pcb boards.
And this may indeed be the case. However if the application involves
differential inputs and outputs its best to have the pair closely
coupled, impedance aside. In that regard broadside is electrically
better if it can be built. Manufactures however tell us otherwise.
Seperating the traces so they are not coupled and then measuring the
impedance across them yields 2*ZO and is easier to calculate. However in
the strick sense of the definition this is NOT differential impedance
because all of the return currents are found in the adjacent planes.
By definition at least some of the return currents need to be in the
trace pair in order to have any kind of differential signaling to
be effective.

The primary reason on a PCB board to have differential signals is the
reduction of EMI. However there are other benefits as well. If the
traces are tightly coupled the pair offers much greater noise emmunity
than single ended traces. Lee Ritchie's paper in PCB Design does a
great job of describing differential IC's functionalities.
Unfortunately his conclusions do not apply to all applications. Low
voltage high frequency signaling tends to lend itself well to
differential routing. Differential signaling works especially well when
other higher voltages that can disturb the signals are around. This
means mixed parts such as LVDS with traditional 5V CMOS. One should not
confuse the requirement of impedance matching with differential
signaling. Unfortunately in the digital world it seems as if they
are the same.

Best Regards,

-- 
Fred Balistreri
fred@apsimtech.com

http://www.apsimtech.com

**** To unsubscribe from si-list: send e-mail to majordomo@silab.eng.sun.com. In the BODY of message put: UNSUBSCRIBE si-list, for more help, put HELP. si-list archives are accessible at http://www.qsl.net/wb6tpu/si-list ****