[SI-LIST] Re: Traces don't cause EMI - really?

  • From: Chris Padilla <cpad@xxxxxxxxx>
  • To: si-list@xxxxxxxxxxxxx
  • Date: Fri, 17 Oct 2003 10:21:16 -0700

Well it has been a LONG time since I posted on this list but I only just 
discovered that my account was in VACATION mode and therefore not receiving 
any postings!  I've been meaning to get back on for the last month or two 
but work kept getting in the way! :)

So to come into the middle of this, I will just comment on was Lee is 
saying and forgive me if I am restating anything anyone else already has:

For a long time, I was under the misconception that high-speed signals 
(busses, clocks, whatever, sharp sub-nanosecond  edges is all I need to 
hear) on outer layers was bad, bad, bad.  They are only bad if not properly 
terminated or poorly routed.  I qualify poorly routed as in excessively 
long or meandering close to noise sources or having lots of layers jumps 
and therefore having what I consider the bane of EMI: vias.

Traces radiate, poorly routed traces can radiate more.  Vias always 
radiate.  Has anyone ever looked at how some horn antennas are fed their 
signal to radiate?  Look into one some time and you'll probably see a very 
short copperish looking metal wire/tube/pin at the very end (or 
beginning).  Does it remind you of a via or a through-hole pin?  Now look 
at the waveguide part of the horn and imagine cutting it in half all the 
way to the feed wire.  Now imagine hammering out the two sections of your 
'cut in half' horn waveguide into two flat planes.  Now they kinda look 
like the planes you find in a multi-layer stack-up of a PCB, don't 
they?  Do you think I could successfully feed my newly shaped waveguide 
with the horn's feed pin?  My efficiency might stink but I won't need to 
couple much energy into the two planes to radiate out and reach my antenna 
to fail CISPR or FCC.

To combat this, some like to stitch gnd vias all around the periphery of 
their PCBs.  This can prevent radiation from the edges of the PCB but it 
will just reflect the energy back into the PCB and could couple it to other 
vias and reradiate out the top/bottom of the board through ICs.  It could 
also make a resonant cavity at some frequency and pray that you aren't 
sending much energy at that frequency!

We measure our fields in dBuV/m.  1 dBuV/m is about 1.1 uV/m!  It doesn't 
take much to fail these tests!

The conclusion is as stated by Lee but I'll add that microstrips, via-less 
microstrips, properly terminated and routed are probably less likely to 
radiate than striplines which, by their nature, will require at least two vias.

Chris Padilla
EMC Engineer
Cisco Systems
San Jose, CA

P.S. BTW, Lee, I am planning to check out your new book...congratulations 
on publishing it!

At 09:33 AM 10/17/2003 -0700, Lee Ritchey wrote:
>What was the setup for the HP experiment?  Over a continuous plane?  If so,
>I question the results.
>
>Everyone who has been party to this discussion on differential pairs used a
>work station or a PC to connect.
>If you look on the back of those products, there is sure to be a sticker
>stating that the box complies with CISPRB and has a CE mark on it.
>
>Open the box and look at the mother board.  You will find that all of them
>have bot outer layers of their mother boards covered with "high speed"
>traces.  Most of them, if not all are single ended signals with a
>combination of series terminations and parallel terminations.
>
>Hows did these boxes pass emissions tests if all of the claims being made
>about traces on outer layers being sources of EMI?
>
>Answer, traces on outer layers that are close enough to a plane to create
>50 ohm transmission lines are not good radiators.
>
>
>Lee
>
>
> > [Original Message]
> > From: Loyer, Jeff <jeff.loyer@xxxxxxxxx>
> > To: <MikonCons@xxxxxxx>; <si-list@xxxxxxxxxxxxx>
> > Date: 10/16/2003 10:12:38 AM
> > Subject: [SI-LIST] Re: Traces don't cause EMI - really?
> >
> > Hi Mike,
> > In your posting, you said:
> > "I designed a special PCB in support of a worldwide seminar tour for =
> > Hewlett-Packard that clearly demonstrated unacceptable (i.e., >FCC Class =
> > B) radiation from single, terminated, 50-Ohm traces on a 10-inch PCB."
> >
> > Just to be clear - are you saying that if I connected 2 properly =
> > designed chips (driver and receiver) together with many properly =
> > designed single-ended transmission lines, they would likely fail FCC =
> > standards?
> >
> > Sorry to force you to restate something that you were so clear about, =
> > but the statement is a bit surprising to me.  My impression has been =
> > that FCC failures were inevitably due to an error in the design - =
> > impedance mismatches, crossing a split plane, changing reference planes, =
> > etc. =20
> >
> > I would expect differential routing to radiate significantly less EMI in =
> > the presence of these errors, but I wouldn't expect a properly designed =
> > board with many single-ended signals to fail EMI.
> >
> > Jeff Loyer
> >
> > -----Original Message-----
> > From: si-list-bounce@xxxxxxxxxxxxx
> > [mailto:si-list-bounce@xxxxxxxxxxxxx]On Behalf Of MikonCons@xxxxxxx
> > Sent: Monday, October 13, 2003 12:20 PM
> > To: si-list@xxxxxxxxxxxxx
> > Subject: [SI-LIST] Re: Traces don't cause EMI - really?
> >
> >
> > In a message dated 10/13/2003 7:17:10 AM Pacific Standard Time,=20
> > leeritchey@xxxxxxxxxxxxx writes:
> > I've tried several times to measure significant emissions from a single
> > transmission line travelling over a plane at the distances above the =
> > plane
> > one uses to create signal paths for logic circuits, the topic of concern =
> > in
> > this thread, with no luck.
> > I welcome measurements from others that supports the statement that =
> > traces
> > over planes are significant sources of EMI.  So far, no one has =
> > presented
> > such evidence.  Lacking such evidence, how can anyone make such claims?
> >
> > True, this thread concerns differential signals, but how are they =
> > different
> > from single ended signals?
> >
> > True, Doug Brooks' paper didn't set out to measure emissions from traces =
> > on
> > outer layers, but it did state that measured emissions were 30+ db below
> > what a mono pole would emit.  =20
> >
> > In all my measurements, the lead frames of the ICs are the big =
> > radiators.=20
> > They make nice antennas.  They stick up above the PCB and they have
> > significant transient currents flowing through them, especially the =
> > power
> > leads.  Check out a PLCC with a near field probe sometime.
> >
> > Time for some measurements from those who want this discussion to =
> > seriously
> > come to any conclusion.  Anyone have any?
> >
> > Lee
> > **************
> > WOW! I just got a chance to review the latest SI list inputs and I'm=20
> > astounded at such comments. Lee, the "evidence" has been around for =
> > decades. The IEEE=20
> > Proceedings published a special edition circa 1989 describing over 40=20
> > different surface structures on PCBs that are efficient antennas, many =
> > of which are=20
> > unintentionally formed by poor trace layouts. I designed a special PCB =
> > in=20
> > support of a worldwide seminar tour for Hewlett-Packard that clearly =
> > demonstrated=20
> > unacceptable (i.e., >FCC Class B) radiation from single, terminated, =
> > 50-Ohm=20
> > traces on a 10-inch PCB. The same board was used to demonstrate both =
> > radiation and=20
> > crosstalk reductions of 6 to 14 dB by the use of guard traces between =
> > signal=20
> > traces (which you recently declared as totally unnecessary). I expanded, =
> >
> > updated, and presented both analyses and confirming measurements at =
> > multiple client=20
> > companies (including IBM, Motorola, AMD, and Johns-Hopkins), and =
> > presented a=20
> > paper at SuperDesignCon 95 illustrating these same effects. IBM =
> > published an=20
> > excellent paper circa 1998 at a Southern California conference (don't =
> > recall=20
> > which) that compared the radiation from traces as a function of their =
> > distance=20
> > from the PCB edges. The bottom line is that ANY trace with current =
> > flowing on=20
> > it generates EM fields and WILL radiate at some levelof efficiency. =
> > That's why=20
> > one should always look to burying high-speed traces unless they are very =
> > short=20
> > relative to the rise time of the signals they conduct.
> >
> > Surface routed differential signal traces offer opposing polarities of =
> > fields=20
> > which tend to cancel, leaving only the effect of a small loop antenna to =
> >
> > radiate (but they still do radiate). That's why I also favor tightly =
> > coupled=20
> > (i.e., closely spaced) pairs for such applications (which, if I recall =
> > correctly,=20
> > you also seem to dislike). Differential pairs are definitely different =
> > from=20
> > individual traces.
> >
> > I have very little time for technical activities (what with the trout =
> > season=20
> > coming to an end soon), but I could not let this thread slip by.
> >
> > Respectfully to all,
> >
> > Mike
> >
> >
> > Michael L. Conn
> > Owner/Principal Consultant
> > Mikon Consulting
> >
> >                          *** Serving Your Needs with Technical =
> > Excellence ***
> >
> >
> > ------------------------------------------------------------------
> > 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 archives are viewable at:    =20
> >               //www.freelists.org/archives/si-list
> > or at our remote archives:
> >               http://groups.yahoo.com/group/si-list/messages=20
> > Old (prior to June 6, 2001) list archives are viewable at:
> >               http://www.qsl.net/wb6tpu
> >  =20
> >
> > ------------------------------------------------------------------
> > 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 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
> >
>
>
>
>------------------------------------------------------------------
>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 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
>

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