I'll add just a few additional points:
1. Differential signalling is typically used when the signal return
integrity through a "single ended ground system" would be ineffective
or would not allow sufficient noise margin to transmit the signal to a
receiver. This is typically the case when there is an expectation of
extremely long signal runs (amplitude loss and potential
electromagnetic intereference), building to building situations
(grounding instabilities) or an expected lossy situation in a much
shorter signalling run which would in essence create the same sort of
conditions which normally would exist in an extremely long signal run.
In very high frequency (fast risetime) situations, such conditions may
exist within a piece of equipment.
2. Since loss and crosstalk have a number of variables that would need
to be considered and both situations would have to deal with these, it
would not be expected that one construction would necessarily be
better than another. Since crosstalk can be affected by the degree of
both capacitive or inductive coupling, affecting the parameters that
would assist in reducing such coupling could yield identical
electrical results in either construction. Losses are about the same.
DC resistance, skin effect losses, and dielectric losses can all be
manipulated, theoretically, and could again yield identical results,
electrically. The actual implementation of these into something one
might design in a particular practical situation might determine the
actual suitability of one construction over the other.
3. In high density applications, while its thought that the BCS
(broadside coupled stripline) might be superior, it does hamper
circuit routing on two layers which might cause problems with the
routing of other signals in the area. While it might be desirable to
limit routing in the differential pair area for crosstalk reasons, the
"high density application" generally makes it impractical to
completely eliminate other signal routing in the area. Again, a
design tradeoff assessment would be necessary to determine if BCS
would work for your particular situation.
4. Since the "effectiveness" of a differential signalling pair scheme
(especially in more difficult signalling situations) is dependent on
the electrical balance of the pair, the construction control of
broadside coupled differential pairs in PCB's can be difficult to
implement such that matched distances between the individual traces in
the pair are equally spaced from a nearby plane resulting in an equal
capacitive loading for each line to "ground" (this assumes equal
dielectric constants in both dielectrics). This can be negated in
large part by sufficient plane distance from the traces in the pair
but then the board thickness increases. Also important is the etched
line widths on each layer and dielectric materials with consistent and
equal dielectric constants would need to be utilized throughout. So
it is not that it cannot be done, it is just more difficult to do in a
production environment. Edge coupled striplines tend to be have less
variables (and therefore less tolerances) to contend with in the
5. As mentioned elsewhere in other comments on this thread, wider
trace widths are needed to keep line impedance stable with regards to
layer registration issues in the BCS construction.
6. Typically, the BCS tends yield a lower impedance for similar
dimensional constructions to ECS (edge coupled stripline). So in a
BCS, larger dielectric distances will be required between the pair
traces and/or reduction of line widths may need to be implemented to
meet certain impedance requirements. In very high frequency
situations, skin effect might have some impact on signals used in
narrower trace widths depending on the actual line width used and the
actual rise/fall time of the signal.
7. The effect of imbalancing the pairs (#4) can produce two
electromagnetic compatibility issues... first, the imbalanced pair
will be more susceptible to stray magnetic fields which are not always
well attenuated in perforate copper plane structures (assuming
stripline construction) even though some eddy current losses (from
field impingement on the planes) will be achieved at higher
frequencies .... (whether that's a problem or not depends on the
system/device noise immunity parameters).... the good news is that
this kind of coupling tends to be "common-mode" and usually can be
rejected by the differential receiver and is the reason why one would
want to make sure the traces in the pair should be closely associated
to one another. Otherwise, the problem can become a "differential
one" and the "protection" is gone... and second, the imbalanced pair
can produce electromagnetic emissions due to a portion of the signal
energy (current) being diverted to areas of the system (larger return
loop area) where it is not intended. In situations where the pair is
tightly coupled to nearby ground planes, it would not be wise to route
such a pair over a plane discontinuity as it would in effect create
the same negative EMC conditions that a single ended trace might do
due to the larger current loop area in the signal return path of the
diverted energy taken from the pair.
Hope that helps!
Michael E. Vrbanac
> 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
> > email@example.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
> > firstname.lastname@example.org. 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
> > email@example.com, firstname.lastname@example.org
> 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
> **** To unsubscribe from si-list: send e-mail to email@example.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 ****
**** To unsubscribe from si-list: send e-mail to firstname.lastname@example.org. 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 ****