Back to the original question:
Yes, it does make a difference which way you route. Check out the eye diagrams
on pp. 27 of the presentation.
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 Curt McNamara
Sent: Wednesday, February 22, 2017 5:17 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%20Pairs.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
