Scott,
Well, not exactly... if that really happened, there would be effects that we
actually do not see in practice i.e. crosstalk to signals on the opposite side
of the plane. I understand the "virtual" thing but it does nothing to explain
how it really works beyond that analogy. Forgive me for being "picky" here but
it is precisely these kinds of things that lead people make incorrect
assumptions. I see this all the time and I try to help fix that wherever I can.
Here's how it really works...
There is mutual inductance and capacitive coupling to the reference plane by
the transmission line definition that creates an out of phase
(reverse) current flow and the planar conductor skin effect/depth keeps it from
co-mingling with other signal return currents on the other side.
That out of phase current flow creates a cancellation field for the source
signal's field produced on the trace above the plane. For the single ended
case, the return current exists in the signal return plane below. For the
differential case, the return current returns in the other signal line in the
pair and the common mode residual generated due to the imbalance of the entire
signaling pair/drivers/loads appears on the plane below. If the rest of the
signaling system is balanced well, failure to couple the differential line
"slightly" to "discipline the pair routing" properly causes increased RF common
mode energy generation simply because there is no meaningful "line balance" and
that is not good for reducing RF emissions.
It's all there and the effects match the theory...
Have a great day!
Michael Vrbanac
EMC Forensics Functional/SI/PI/EMC Design Austin, TX
On 07/06/2016 10:25 AM, Scott McMorrow wrote:
Because of the magic of the image plane.
The image plane already causes far field cancellation for microstrip.
Essentially, on a microstrip with a 4 mil dielectric, the virtual
equal and opposite image trace is 8 mils away. It's like operating
two dipole antennas 180 degrees out of phase at a spacing of 8 mil.
They pretty much cancel each other out.
Scott McMorrow
Technical Director SI/PI
16 Stormy Brook Rd
Falmouth, ME 04105
(401) 284-1827 Business
http://www.teraspeed.com
On Wed, Jul 6, 2016 at 11:18 AM, Jeff Loyer <jeff.loyer@xxxxxxxxxx> wrote:
Something that I’ve wondered about is: If microstrip (or stripline)------------------------------------------------------------------
might cause EMI, how come Intel never saw any significant difference
when they went to differential busses between processors? Intel
replaced the single-ended front-side bus (high EMI) with differential
signaling (low
EMI) for communication between the processors and memory controller
and yet I’ve never heard anyone write (or remark) that this made an
impact on the EMI signature of their servers or desktops.
*Jeff Loyer*
*From:* Sanjeev Gupta [mailto:sanjeev@xxxxxxxxxxxxxxxxxxxxxxxxxx]
*Sent:* Wednesday, July 6, 2016 6:06 AM
*To:* istvan.novak@xxxxxxxxxxx
*Cc:* doug@xxxxxxxxxx; si-list@xxxxxxxxxxxxx; Jeff Loyer; Lee Ritchey
*Subject:* Re: [SI-LIST] Re: Via fence along board edge
I have another question to EMI experts on the same lines and add few
more points in the discussion..
Which is good from EMI point of view.. stripline or microstrip routing?
I conducted few EMI simulation experiments long time back and found
something interesting.
experiment was related with microstrip vs stripline radiation using
3D EM tool in real PCB condition and measured far-field@3m .
I found stripline radiation much higher than microstrip. This is
definitely not consistent with established myths..Normally stripline
is supposed to be better than microstrip routing for EMI. But, any
stripline routing in real PCB will come with at least 2 via
transition to make connection with components.
The conclusion was pointing towards that any via-addition in the
layout will create good amount of radiation. Therefore, stripline
radiation was worse than microstrip.
I am not sure how does this conclusion will apply to GND via
stitching fencing and ongoing discussion. But, any via addition in
the layout does not seem to be free insurance.
Another simulation experiment was related with radiation through
bends (90degree, 45 degree,45 degree mitred). I could not find any
difference in radiation till 10GHz. difference was marginal beyond
10Ghz. So 90 degree bend radiation is also a myth. Many earlier
discussion on si-list also confirms the same conclusion.
it is not possible to simulate the absolute EMI radiation from given PCB.
But relative EMI assessment for different layout condition is
definitely possible.
Thanks
Sanjeev
SigIntegrity Solutions
www.sigintegrity-solutions.com
------------------------------------------------------------------
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:
//www.freelists.org/webpage/si-list
For help:
si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field
List forum is accessible at:
http://tech.groups.yahoo.com/group/si-list
List archives are viewable at:
//www.freelists.org/archives/si-list
Old (prior to June 6, 2001) list archives are viewable at:
http://www.qsl.net/wb6tpu
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:
//www.freelists.org/webpage/si-list
For help:
si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field
List forum is accessible at:
http://tech.groups.yahoo.com/group/si-list
List archives are viewable at:
//www.freelists.org/archives/si-list
Old (prior to June 6, 2001) list archives are viewable at:
http://www.qsl.net/wb6tpu
