From: Michael Khusid (firstname.lastname@example.org)
Date: Wed Jan 17 2001 - 11:45:12 PST
If your board is so dense, I would increase coupling between the legs of
your differential pair, i.e. I would place them closer to each other.
Microstrip differential pair with 5 mil lines, 5 mil spacing between legs on
4.5 mil core (that's the standard size for GETEK core if I recall
correctly?) will get you 100 Ohm differential impedance. That would be a the
edge coupled solution, i.e. legs on the same layer. There are also broadside
coupled solutions, i.e. lines on different layers one under another.
The crosstalk between legs of differential pair can be used to your
advantage, that will keep the energy of the signal between those lines.
If you'd like to decrease the crosstalk between differential pairs, use
larger spacing between differential pairs, while using smaller spacings
between lines of the same differential pair. I've seen this issue to come up
with some board designers who try to keep the same spacing between *all*
lines on the board.
Sitara Networks, Inc.
> -----Original Message-----
> From: email@example.com [mailto:firstname.lastname@example.org]
> Sent: Wednesday, January 17, 2001 1:43 PM
> To: email@example.com
> Subject: RE: [SI-LIST] : Z Odd-mode, edge-coupled, 50ohms?
> Hi all,
> Then... Could someone please tell me (any guidance is
> appreciated) in
> layman's terms how I "might" route the differential traces, #1 using
> microstrip; and #2 doing it stripline. I'm working a board with GETEK
> material, it has a couple .1mm BGAs and many, many, many differential
> pairs. I've done some preliminary calcs (using Polar Instr. CITS
> software), and come up with .008" lines with .008 spacing and .024"
> spacing between the pairs, routing on the microstrip layers.
> I'd like to
> go smaller, and possibly decrease the dielectric to the plane
> layer, but
> I've heard there "might be" crosstalk problems. Anyone?
> I'm especially interested in routing these on stripline
> layers, but I've
> heard that's not a good practice either. Help?
> "This is just the beginning..."
> Thanks for all your help.
> Sr PCB Designer
> San Diego, CA
> (P.S. I've got most all the articles I need, from Lee Ritchey's to
> Mentor's App note, to Eric Bogatin's stuff to UltraCad's stuff, etc.
> etc., but I need something in PCB layout terms. Thanks)
> ---------Included Message----------
> > Date: Wed, 17 Jan 2001 09:58:42 -0800
> > From: "Neffody Kraskoff" <Neffody.Kraskoff@Plexus.com>
> > Reply-To: "Neffody Kraskoff" <Neffody.Kraskoff@Plexus.com>
> > To: "'firstname.lastname@example.org'" <email@example.com>
> > Subject: RE: [SI-LIST] : Z Odd-mode, edge-coupled, 50ohms?
> > Hi Mitch,
> > What type of driver technology are you using, is it
> LVDS? If so
> then LVDS
> > traces are 100ohm differential.
> > If the 100ohm terminating resistor connects to the pos and neg
> signals of
> > your differential pair like so:
> > -------------DIFF_sigP---------.---load pin (device)
> > |
> > /
> > \ 100ohm R
> > /
> > |
> > -------------DIFF_sigN---------.---load pin (device)
> > Then your required trace impedence must be 100ohms
> (matches the
> > resistor value).
> > Its extremely unusual to have 50ohm single-ended lines on the
> same trace
> > layer with 50ohm differential. Usually, its 100ohm
> and 50 ohm
> > single ended.
> Tired of limited space on Yahoo and Hotmail?
> Free 100 Meg email account available at http://www.dacafe.com
> **** To unsubscribe from si-list or si-list-digest: send e-mail to
> firstname.lastname@example.org. In the BODY of message put: UNSUBSCRIBE
> si-list or UNSUBSCRIBE si-list-digest, for more help, put HELP.
> si-list archives are accessible at http://www.qsl.net/wb6tpu
**** To unsubscribe from si-list or si-list-digest: send e-mail to
email@example.com. In the BODY of message put: UNSUBSCRIBE
si-list or UNSUBSCRIBE si-list-digest, for more help, put HELP.
si-list archives are accessible at http://www.qsl.net/wb6tpu
This archive was generated by hypermail 2b29 : Tue May 08 2001 - 14:30:38 PDT