John Lark>> >>
>>> Hi
>>>
>>> I am designing an 8 layer board with a Virtex 4 device on it. I will have
>>> 2 solid ground planes and 2 split power planes. If I have a signal plane
>>> that is between a ground and power plane will it matter if I cross a split
>>> on the power plane with a signal track. I know that you should not cross a
>>> split it in a plane if you are referencing to that plane. But if I have a
>>> solid ground plane beneath the track will it use this plane as its
>>> reference rather than the power plane.
>>>
>>> Cheers
>>>
>>> Jon
>>
>> No, it doesn't matter. The strange concept of "reference planes" is
>> irrelevent here... how does the signal know what plane you think it's
>> referenced to?
>>
>> If the power planes are bypassed well enough to make them reliable
>> power sources, then they are AC equipotential with the ground plane,
>> so the signal sees them all as ground. And a small slit in a power
>> plane is essentially invisible for edges slower than a few 10's of
>> picoseconds.
>>
>> John
>
>John,
>
>You're the only person who I won't directly challenge on your assertion
>because of your experience in producing quality products while
>confronting these types of issues directly.
>
>Suffice it to say that "today's common theory" suggests crossing the
>split in the specified case - like crossing any split - can be the root
>of crosstalk and EMI issues in addition to signal fidelity issues, just
>to a lesser extent than for signals on the outside layers.
>
>I'd love to be able to wrap my mind around how crossing this split
>wouldn't affect the signal in measurable ways, but the things I've been
>taught - my "faith" perhaps - suggests otherwise. I was once of a mind
>where crossing the split would be a non-issue but was brought over to
>the dark side with convincing arguments that tied in mith my more
>fundamental understanding of transmission line theory.
>
>- John_H
ground============================================================
signal------------------------------------------------------------
power ======================== =================================
whatever ========================================================
OK, there's a slit in the power plane. It's probably about as wide as a normal trace width, call it 8 mils. Let's say the plane-plane spacings are similar distances. Both halves of the split power plane are bypassed to the ground plane by real capacitors and by the considerable large-area plane-plane capacitance.
In order for the trace impedance to change as the trace cruises over the gap, the potential in the middle of the gap would have to be non-zero. But the electric field from the signal trace can hardly penetrate through the gap... that's simple electrostatics. The signal sees uniform ground above, and a slightly lower dielectric constant below, in the gap region. That raises the trace impedance a tiny bit just above the gap, for a tiny distance. The "reference plane" issue is silly, as all the planes are at AC ground.
I've built and TDR's such structures to better than 30 ps resolution. A reflection from such a gap is lost in the normal impedance noise, caused by thickness variations and the glass weave in the board. In the nanosecond domain, it's totally invisible.
On a 2-sided board, a microstrip trace on one side and a cut ground plane on the other,
signal-----------------------------------
ground================== ==============
a narrow slit in the ground plane is still a tiny impedance discontinuity on a TDR plot.
All this "reference plane" stuff is ludicrous. It sure ain't "transmission line theory", it's folklore.
John