[SI-LIST] Re: Does power/ground pair edege radiation noise really matter in the EMI test?
- From: steve weir <weirsi@xxxxxxxxxx>
- To: LIU Luping <liuluping@xxxxxxxxxx>
- Date: Mon, 27 Dec 2010 20:29:42 -0800
LIU Luping wrote:
> 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.
>
The information is insufficient. When you say that the PI performance
is similar:
* Is that similar at the die?
* Is it similar as measured at certain test points attached to the power
cavity?
* Is it similar as measured at some unpopulated bypass capacitor location?
* Is it similar as measured at some populated bypass capacitor location?
Are there polygons joining the capacitor via connections and the IC via
connections, or are the capacitor connections to the IC power/gnd vias
made with traces?
The edges form a discontinuity. Some portion of the energy escapes from
the edges, while much of it reflects back into the cavity. If you have
noise problems and want to fix them with minimal parts and / or design
changes, then you need to understand what is conveying the noise. For
example: Do you see the extent of the problems change when you relocate
cables, or rotate the PCB?
If you are just trying to patch over a compliance problem and need to
get to an answer quickly, then thinning out the dielectric is often a
big help.
>
> 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?
>
>
Anything that is not lossy will push the resonances around in frequency
and location of the modal peaks, rather than get rid of them. The only
way to get rid of the energy is with real loss. Depending on the
design, you have different options as to how to go about moving the
energy in frequency and/or location and/or getting enough loss before
the energy couples to something that ultimately conveys energy to the
outside world.
> 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
>
>
>
>
--
Steve Weir
IPBLOX, LLC
150 N. Center St. #211
Reno, NV 89501
www.ipblox.com
(775) 299-4236 Business
(866) 675-4630 Toll-free
(707) 780-1951 Fax
------------------------------------------------------------------
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:
