There are probably many different expensive solutions out there.  But, if you
only need to transfer the signal 1 inch, a cheap solution which might work could be a
high density flex connector.  Get a 2 sided shielded flex cable with around 4
internal conductors.  Use the middle 2 for the differential signal while grounding
the outer 2 &, or course, ground the shield.  I've successfully transferred a 4GHz
signal with such a setup.

When I say high density flex, I'm talking 0.5mm pin-pin.  The really thin traces on
the flex help keep capacitance & radio emitions down.

____________
Brian Guralnick


----- Original Message -----
From: "Brad Velander" <[EMAIL PROTECTED]>
To: "'Protel EDA Forum'" <[EMAIL PROTECTED]>
Sent: Wednesday, December 05, 2001 8:59 PM
Subject: Re: [PEDA] 50 ohm differential impedance connections and traces


| Scott,
| I can give you an answer, however your engineers may choose to not
| accept it. It is from one of the preeminent figures in signal integrity, Lee
| Ritchey, it published in the March 1999 PCD magazine.
| Contrary to popular belief you do not have to deal with differential
| impedances in your PCB traces. This is the fallacy of this design dilemma.
| The simple solution is two equal length (+/- 500 mils) singular controlled
| impedance lines routed along roughly the same path. The two lines should
| each have an impedance to Gnd of 1/2 Zo or 25 ohms. Each trace should be
| terminated to Gnd in it's characteristic impedance. Voila, you have a 50 ohm
| balanced impedance differential pair.
| Your calculations are definitely out there, I don't know how you
| have been calculating this figure but here is my solution using your basic
| characteristics. Dielectric thickness: 0.008 inches, total copper weight: 1
| oz (0.0014in), FR4 (Er - 4.7).
|
| Your trace width should be 27.5 mils (0.0275 inches). Don't forget to
| terminate each line with a 25 ohm terminator.
|
|
| If you need a copy of the article, let me know, I will scan it and
| forward it to you.
|
| Sincerely,
| Brad Velander.
|
| Lead PCB Designer
| Norsat International Inc.
| #300 - 4401 Still Creek Drive,
| Burnaby, B.C., Canada, V5C 6G9.
| Tel   (604) 292-9089 (direct line)
| Fax  (604) 292-9010
| Website: www.norsat.com
|
|
| -----Original Message-----
| From: Scott Ellis [mailto:[EMAIL PROTECTED]]
| Sent: Wednesday, December 05, 2001 4:17 PM
| To: Protel EDA Forum
| Subject: [PEDA] 50 ohm differential impedance connections and traces
|
|
| A couple of questions.
|
| Does anyone have a good way of doing board  to board connection (only about
| an inch) for a differential 50 ohm connection?
|
| Can I make two parallel connections with 100 ohm twisted pair?
|
| We have done some calcs for a FR-4, 1 oz copper, double sided, 1.6mm thick,
| and we get traces 140thou, 8thou spacing over a gound plane for a 50 ohm
| differential impedance. Can anyone confirm our result? 140 thou is getting
| up there!
|
| The reason for the questions is that we need to take a differential PECL
| signal from one board to another and maintain the signal integrity.
|
| Scott Ellis
| Manager
| Novatex Research - Excellence in Electronic Research & Development
| [EMAIL PROTECTED]
| 41 Yule Road, Merewether, Newcastle, NSW 2291, Australia
| Ph 0412 988408   Fax 02 49636058
|
|

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
*
* To leave this list visit:
* http://www.techservinc.com/protelusers/leave.html
*
* Contact the list manager:
* mailto:[EMAIL PROTECTED]
*
* Forum Guidelines Rules:
* http://www.techservinc.com/protelusers/forumrules.html
*
* Browse or Search previous postings:
* http://www.mail-archive.com/proteledaforum@techservinc.com
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to