[SI-LIST] Re: risetime effects of plane breaks

Scott,
Excellent summary. That was my concern on striplines crossing with a bus
rather than individual signals. In a way, it is like wire bond signal leads
without the ground leads mixed among them. The signals start referencing
each other instead. Or you can see it as a trade-off between adding
shielding layers or spreading the bus spacing (decreasing routing channels)
in a high density/performance design. My own rule of thumb is space them at
least equal or larger than the gap itself when crossing. That's is at least
a 3x decrease in routing channels so it is quite costly and has to be weight
against adding shielding layers. Sometimes its worth it, sometimes its not.
As for EMI, if you dig back some discussion I had with Steve, I always
prefer solid ground planes referencing microstrips on top and bottom of PCB
and then stitch the edges with ground vias. Hopefully any of those excited
noise on the cut power planes will be trapped inside.

-----Original Message-----
From: Scott McMorrow [mailto:scott@xxxxxxxxxxxxx]
Sent: Thursday, January 20, 2005 2:39 PM
Cc: Si-List
Subject: [SI-LIST] Re: risetime effects of plane breaks


When this thread started I was on vacation.  However, I found this 
interesting enough to resurrect some previous simulations I'd performed 
in CST Microwave Studio.  After much playing, twiddling and generally 
having fun I can say several things:
1) It's pretty easy to confirm Doug's results using 3D fullwave 
simulation. In fact, in about 30 minutes I can replicate his case and 
create a design that can be easily modified for many other 
possibilites.  The microstrip split plane crossing is a no-brainer.  
Just don't do it and expect anything approaching an EMI "clean" system.

2) Chris and Steve ... and eventually myself, wanted to know more about 
the various different stripline plane crossing configurations, so I 
setup a simulation with a VDD island not unlike what might be found in a 
memory system, and performed multiple simulations with dual asymmeteric 
stripline crossing the plane twice on it's way to the memory module. Not 
surprisingly the following is true:

    It is best not to cross a split plane ... even with stripline.
    If you do, it is better to cross a split that is adjacent to a
    ground plane
    It is even better if you cross a split adjacent to a ground plane on
    the stripline layer furthest away from the split plane (i.e. next to
    a ground plane)
    It is worst to cross a split plane that has no adjacent ground.
    The width of the gap in the plane makes very little difference until
    it becomes really small or really big.
    Crosstalk scales almost linearly with the number of aggressors
    crossing the split. (i.e. - it can get really bad!)
    Bypass of the split power island helps for frequencies below 500
    MHz, provides no help for frequencies higher than 500 MHz, and as
    such has no benefit to most of the noise and crosstalk created by
    high speed signals crossing onto and off of the island.

The energy released into the power/ground plane cavities by high speed 
signal split plane crossings is huge and essentially cannot be 
suppressed with bypass capacitors.  Any attempt at supprerssion with 
capacitors exhibits what I call a "Whack-A-Mole" property.  You can 
never get rid of those pesky little moles. All you can do is to move 
them around by thumping them. Given that all this energy is rattling 
around the PCB power planes from split plane crossings, it will 
eventually go somewhere.  Since it's really easy to develop all sorts of 
resonant power island cavities that have primary resonant frequencies in 
the 500 MHz to several GHz range, it is not at all unlikely that any 
split plane crossing has an extremely strong potential to excite a 
resonance in a frequency range that will cause most systems to fail EMC 
compliance testing  About all you can do is to shield the cavity patches 
using ground layers.  This should reduce the radiated energy 
significantly, but will not totally eliminate it, since eventually it 
will find it's way to all those pesky device and package leads.


best regards,

Scott

-- 
Scott McMorrow
Teraspeed Consulting Group LLC
121 North River Drive
Narragansett, RI 02882
(401) 284-1827 Business
(401) 284-1840 Fax

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
  
------------------------------------------------------------------
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: