[SI-LIST] Re: 90 degree bend

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:
http://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:     
                http://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: