PCB Impedance Control

John Larkin wrote:
(snip)

> If a diff signal hits a region where the impedance changes, there will
> be a partial differential reflection, kicked back to the driver.
> Unless the driver is a matched impedance, which it generally ain't,
> the reflection will bounce off the driver and get tangled with the
> data stream, introducing jitter and closing up the data eye.

That is true, but it is separate from the question of crossing
planes.

> The differential impedance is determined by both signal-ground
> capacitance and signal-signal capacitance (which gets double credit).
> For a very fast edge, a diff signal that changes layers on vias can
> encounter a different impedance region and do some bouncing. The fast
> parts of the signal will tend to bounce back, and the slow parts will
> tend to pass forward, not good. The via structure can certainly be
> optimized for signal integrity. Above a few hundred ps risetime, it's
> generally not a big deal.

The length of the impedance discontinuity could (or should) be
very short.  If it gets back to the right impedance on the
other side, the reflections will cancel.  Again, separate from
the question of split planes.

-- glen

Symon wrote:
(snip, someone else wrote)

>>The signal is differential so when the return currents hit the wall, they 
>>cancel each other out at that border.  There's no reflection because the 
>>common mode voltage isn't changing.  If the differential signal wasn't 
>>routed differentially, then the reference currents would disperse when 
>>they hit the discontinuity and then eventually find each other or other 
>>ways to balance the current.  Even though a large portion of the reference 
>>current is in the plane, the discontinuity results in almost no distance 
>>to travel for the differential reference currents to find peace.

That depends on good board layout, but should be true.  Especially
one should be sure that the capacitance (per unit length) from the two
to ground are equal.

> A good point, I agree, that's true. As you say, there will be a 
> discontinuity nevertheless, as the currents need to cancel out across the 
> plane, but I would think this is a small effect. Furthermore, in that case, 
> I think it means it is important to match the lengths of the traces from 
> each termination to the vias as well as the total length of the individual 
> traces. In the case where the extra ground vias are in place, that isn't so 
> important.

For a true differential signal the ground plane current is perpendicular
to the signal wires.  Yes, that does depend on the conditions being
close enough to the same for the two wires.

> Of course, the differential signal continues on its merry way through the 
> vias. Without the ground vias, the transmission line impedance will have a 
> significant discontinuity.

It is important that the impedance be the same on both sides.  The
length of the via itself should be much less than the wavelength,
and so should have a relatively small effect.

I was thinking of the case where the signals stay in the same layer,
but switch reference planes.  If one is careful with the edges of the
planes, it should be possible to minimize the discontinuity.

-- glen

John Larkin wrote:

(snip)

>>Consider a sphere with no other metal objects around it.
>>Add some charge and compute the change in voltage.
>>Divide, and that is the capacitance.  It is a little harder
>>to calculate for other shapes, but it is still there.

> 1 cm radius is 1 pF!

In CGS units the unit of capacitance is cm.
(resistance is s/cm and inductance s**2/cm.)

-- glen

>
> Bizarre. This guy can't even afford real pc boards, so has to fake it
> with wire and old copperclad. Fig 3 is hilarious; of course a signal
> radiates more on the side it's exposed to the antenna. Of course vias
> are inductive discontinuties.

On the assumption that people aren't trolling, and to save people's
time I would suggest that the Signal Integrity mailing list is perhaps
a better place to continue. Everyone on that list has an interest in
SI, so perhaps a more informed debate can continue.
(Note: this is not saying that John or the other side is incorrect,
just a suggestion)

See http://www.freelists.org/list/si-list for the web interface.

Andrew