Curt,
Great presentation. Agreed - thanks!
To further supplement. If loss and edge-rate degradation is a concern, then
roughness of the copper may need to be considered as well, since it will
attenuate the higher frequency harmonics more so than just dielectric loss.
You you will need a more complicated field solver to deal with conductor
loss due to roughness.
Also fiber-weave effect should be considered when designing the stack-up to
mitigate intra-pair P/N skew. Much has been written on fiber-weave effect
over the last few yrs and there were some great papers at this year's
DesignCon (and last year's too) on the subject. I touched on it a few years
ago here:
https://blog.lamsimenterprises.com/2011/01/08/fiber-weave-effect-timing-skew
/
-Bert
Bert Simonovich
Signal/Power Integrity Practitioner | Backplane Specialist | Founder
LAMSIM Enterprises Inc.
Web Site: http://lamsimenterprises.com
Blog: http://blog.lamsimenterprises.com/
-----Original Message-----
From: si-list-bounce@xxxxxxxxxxxxx [mailto:si-list-bounce@xxxxxxxxxxxxx] On
Behalf Of Curt McNamara
Sent: 22-Feb-17 6:17 PM
To: dmarc-noreply@xxxxxxxxxxxxx; lists@xxxxxxxxxxxxxx; si-list@xxxxxxxxxxxxx
Subject: [SI-LIST] Re: differential or single-ended PCB routing for cabled
input and probed output?
Great answer.
However, there are some small differences between loose and tight coupling.
The first 30 pages of this presentation give an overview of some of the
issues.
http://www.westmichigan-emc.org/archive/2014%20IEEE%20Bill%20Spence%20Diff%2
0Pairs.pdf
Curt
Curt McNamara, P.E.
Engineering Consultant
612.305.0440 x248
www.npe-inc.com
-----Original Message-----
From: si-list-bounce@xxxxxxxxxxxxx [mailto:si-list-bounce@xxxxxxxxxxxxx] On
Behalf Of Bert Simonovich
Sent: Wednesday, February 22, 2017 4:58 PM
To: lists@xxxxxxxxxxxxxx; si-list@xxxxxxxxxxxxx
Subject: [SI-LIST] Re: differential or single-ended PCB routing for cabled
input and probed output?
Gary,
Technically it doesn't matter. As Lee often says there is no such thing as a
"differential trace". A "differential pair", on the other hand is merely 2
traces driven differentially. They can be routed together with wide
separation, meaning they are uncoupled electromagnetically (i.e. 2
single-ended), or routed closer together with coupling. A field solver is
needed to determine the final differential impedance. When Zodd = Zeven,
they are no longer coupled together and Zodd = the characteristic impedance
of a single trace (Zo). The differential impedance, Zdiff = 2*Zodd. If your
field solver does not give you Zdiff directly, you can find a little more
detail in an article on my blog site on how to get it from RLGC matrix:
https://blog.lamsimenterprises.com/2011/02/07/pcb-cross-sectional-geometries
/
If you design for close-coupling diff-pairs, then when you split and run
single-ended to SMA connectors for instance, you need to adjust the line
width accodingly to make sure the single-ended trace impedance equals the
odd mode impedance of the close-coupled differential pair.
Regards,
Bert Simonovich
Signal/Power Integrity Practitioner | Backplane Specialist | Founder LAMSIM
Enterprises Inc.
Web Site: http://lamsimenterprises.com
Blog: http://blog.lamsimenterprises.com/ ;
-----Original Message-----
From: si-list-bounce@xxxxxxxxxxxxx [mailto:si-list-bounce@xxxxxxxxxxxxx] On
Behalf Of Gary Giust
Sent: 22-Feb-17 3:36 PM
To: si-list@xxxxxxxxxxxxx
Subject: [SI-LIST] Re: differential or single-ended PCB routing for cabled
input and probed output?
I stand corrected. PCIe4 requests a differential trace on the PCB (so I'll
adopt that).
That said, I've often wondered about a similar question. Not considering any
standards, If you're designing a board for a chip having a differential
output that connects to a pair of SMAs to view each conductor in a separate
scope channel (to view crossing voltage, for example), should the signal on
the board be routed using differential or single-ended traces (or, it
doesn't matter)?
On 2017-02-22 12:01, Gary Giust wrote:
I'm creating a board that inputs a differential signal using SMA------------------------------------------------------------------
connectors on one side, and passes the signal through 12" of PCB trace
before terminating each trace with a 2 pF capacitor to ground. I'll
(active) probe each of the differential conductors single-endedly
(using
2 channels of a real-time scope, one channel for each conductor).
DUT---SMA cables---12" trace---probe pads---2pF caps---ground
Should the traces be routed as (1) differential or (2) single-ended on
the PCB?
Since the measurement is single-ended, and the input to the board is
cabled, I'm thinking they should be routed single-ended on the board
as well. If the traces are routed differentially, I believe they'll be
an impedance mismatch when the signal hits the differential PCB
routing, which can be avoided by routing single-ended.
Does that sound about right?
------------------------------------------------------------------
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
