[SI-LIST] Re: 90 degree bend
- From: Scott McMorrow <scott@xxxxxxxxxxxxx>
- Date: Mon, 30 Aug 2004 12:47:33 -0400
Alright newbies, the electron-as-marbles theory of 90-degree bends
really does not fly. (Pun intended.) What is propagating down a trace
is an electromagnetic wavefront, not physical electrons. Please go back
to your Electromagnetic and Physics textbooks.
As for 90 degree bends, the impact that these have on signals is limited
by the width of the trace and the Er of the material used.. Microwave
boards often have very wide traces on very thick substrates. Excess
capacitance (or excess inductance, depending on the frequency being
analyzed) is proportional to the length of the corner discontinuity. A
100 mil trace, as might be used in a microwave design, will have a
discontinuity length of 1.414 X 100 mil or 141 mils. On a ceramic
substrate with an Er of 10, this leads to an electrical length of about
33 ps, which is a big delay error and a big impedance bump which causes
high insertion loss at some high frequencies. However, for digital
boards where traces tend to be relatively narrow, the length of these
corners is small, say 14 mils, for a 10 mil trace width, limiting the
discontinuity and delay error to 2 ps or less. A 5 mil trace would have
a potential delay error of about 1 ps/corner.
Now a 1 or 2 ps delay error might be considered a problem by some, but
there are some mitigating factors:
1) All modern-day PCB CAD tools mitre corners, eliminating 90 degree
bends, and reducing the overall corner error by a significant amount.
Let's just say there is about a 4:1 reduction in the delay introduced
for starters. Thus, for a 5 mil trace this would limit the delay error
to 250 fs, which I defy most of you to measure accurately. (Please do
not confuse this with any additional skew introduced by serpentined
trace coupling, which can also introduce additional delta skew.)
2) Most digital boards are fabricated with FR-4 or other
fiberglass-epoxy laminate materials. These materials have significant
global and local Er variations, due to trace orientation over the
underlying weave, which can account for a 2 to 4 ps/in delay variaiton
between any two traces on an FR-4 PCB. As a result, any delay due to
corner bends tends to be insignificant when compared to other sources of
trace delay error.
As a result, corners are just not that interesting any more.
best regards,
scott
>
>
>
--
Scott McMorrow
Teraspeed Consulting Group LLC
121 North River Drive
Narragansett, RI 02882
(401) 284-1827 Business
(401) 284-1840 Fax
(503) 750-6481 Cellular
http://www.teraspeed.com
Teraspeed is the registered service mark of
Teraspeed Consulting Group LLC
------------------------------------------------------------------
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 FAQ wiki page is located at:
http://si-list.org/wiki/wiki.pl?Si-List_FAQ
List technical documents are available at:
http://www.si-list.org
List archives are viewable at:
//www.freelists.org/archives/si-list
or at our remote archives:
http://groups.yahoo.com/group/si-list/messages
Old (prior to June 6, 2001) list archives are viewable at:
http://www.qsl.net/wb6tpu
Other related posts:
