[SI-LIST] Re: Does power/ground pair edege radiation noise really matter in the EMI test?
- From: LIU Luping <liuluping@xxxxxxxxxx>
- To: Jory McKinley <jory_mckinley@xxxxxxxxx>, Lee Ritchey <leeritchey@xxxxxxxxxxxxx>, steve weir <weirsi@xxxxxxxxxx>
- Date: Tue, 28 Dec 2010 12:10:52 +0800
Dear all:
Sorry for mistake operation and much appriciate for your replies.
Shall we conclude that the answer to this question is YES, although still some
puzzles:
As Istvan and Brad replied,we can separate this problem into two case:
1) Power plane on the outside of the board stackup,e.g. microstrip type,may be
treated as
Patch antenna and expect to radiate bit more energy than the striplines
mode(case 2),but the
noise source seens not directly from the eedge radiation,as Lee Ritchey
recommand:
Pantic-Tanner, De. Zorika etal, "Radiation Edge Effects in PCBs, (20H rule),
San Francisco State University, May 2000.
We have a test digital board with power/ground pair (4mil core) on the 2/3
layer of a 8 layers board, all decouple capacitor
mount on the top side with few hundreds mils distance from the power pin of the
chip,have similar PI performance with a
compare board which the power/ground pair in side the stackup and the decap
mount on the bottom side,but the RE test shows
5~10dB difference from hundreds to 3GHz,include the 375 MHz and higher.
Should we pay attention to the edge noise here? it seens nothing to do with
this noise source,stich GND via is not effective now.
2)Power plane inter side of the board stackup,e.g.stripline type. many comments
here,especially on the excite souce(signal line/via/SSN,etc.),
the coupling path, and the edge radiation mechanism,all have different
views,and the solution,.
From the excite souce,the parasitic inductance of via will consist an natural
filter that isolate most of these noise into the plane.
Due to the presence of via and trace,prediction of edge radiation levels
using antenna models rarely produces accurate results.
As for the solution,stich GND via may be not so perfect,one of the reason is
the edge connector,then not all four sides can be grounded,
and it need two GND plane at top and bottom side; another reason is that the
reflections from the edges reflect back into the PCB, increasing
the magnitude of internal resonant peaks and secondary coupling backonto traces
and vias. The coupling can be significant enough to create
signal integrity problems such as ground bounce and simultaneous switching
output (SSO) noise.
Am I right?
Best Regards,
LIU Luping
*****************************************************************
This e-mail and its attachments contain confidential information from
HUAWEI, which is intended only for the person
or entity whose address is listed above. Any use of the information contained
herein in any way (including, but not
limited to, total or partial disclosure, reproduction, or dissemination) by
persons other than the intended recipient(s)
is prohibited. If you receive this e-mail in error, please notify the sender by
phone or email immediately and delete it!
***********************************************
----- Original Message -----
From: Jory McKinley
To: Lee Ritchey ; steve weir
Cc: Istvan Novak ; liuluping 41830 ; si-list@xxxxxxxxxxxxx
Sent: Tuesday, December 28, 2010 6:10 AM
Subject: Re: [SI-LIST] Re: Does power/ground pair edege radiation noise
really matter in the EMI test?
Hello Lee,
We have a case in which an existing customer design was not functioning due
to one direct path to path coupling in the PLL. This path to path coupling was
one resonate structure path (resonate at critical PLL frequency) to the PLL
power path. We came in and found the amount of coupling was in the -20dB range
which based on PLL simulations should have been less than -50dB at this
critical frequency. We caught this path on the old package (plus some others
not related in separate blocks ) and spun a new package with coupling below the
-50dB target. The re-spun package is fully functional to date and trying to
get customer permission to turn into a paper.
There are other cases and admittedly more the common as you point out in
which it is less clear as to what the exact coupling path that has created
issues with a product. For example, we are working on which shows at least 5
coupling paths that are individually close to the allowable coupling but
collectively sum above the absolute maximum coupling. Of these paths one of
them has a resonate in the frequency of interest which to be safe we took care
to damp this path while trying to further isolate the others.
Regards,
-Jory
------------------------------------------------------------------
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 technical documents are available at:
http://www.si-list.net
List archives are viewable at:
//www.freelists.org/archives/si-list
Old (prior to June 6, 2001) list archives are viewable at:
http://www.qsl.net/wb6tpu
Other related posts:
