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

  • From: MikonCons@xxxxxxx
  • To: leeritchey@xxxxxxxxxxxxx
  • Date: Sun, 1 Feb 2004 15:30:03 EST

In a message dated 2/1/2004 9:35:10 AM Pacific Standard Time, 
leeritchey@xxxxxxxxxxxxx writes:
Wow!  This topic keeps coming up.  Wasn't so long ago that we had a very
long exchange where proponents of this notion provided the research papers
that  supported it.  I got copies of all of them and looked for some
objective measurement of the EMI caused by a trace routed on an outer layer
over a plane and then moved below the plane.
None of the papers did such an experiment in a way that could be used to
bet money on.  I pointed out that the real source of EMI from a PCB were
the lead frames of components that stick up from the PCB.  While at Maxtor,
we had this very problem with disc drives.  We fixed the problem by
changing lead frames from PLCCs to QFPs- packages that don't stick up very
far from the PCB.  If you want to see this in action, go to Frys or any
place else that sells stand alone disc drives and look at how the PCBs are
designed.  All of the signal traces are on outside layers and all of the
disc drives comply with CISPRB B.

We used a pedicel of equipment that allowed the PCB to be laid on it and
then scanned to provide a 2D picture of where emission were coming from.  I
cannot remember the name of the tool, but it had a table with a grid on it
on which the PCB was mounted.  The output looked a lot like what one gets
from a thermal mapping tool showing places with higher emissions.  The
sources of EMI were very clear- the IC lead frames.
Thanks, Lee, for including me on your distribution. 

I absolutely agree that high-speed boards can be designed with many traces on 
the PCB surfaces IF there is a high integrity enclosure. 

The tool you mentioned was likely of thick, planar construction with many 
separate pickup coils in a grid. I have seen several test labs with this tool. 
you indicated, the lead frames DO radiate substantially. Assuming buried PCB 
traces, some of this radiation can be cancelled by routing the lead pad back 
under the package before dropping the via. Aside from that, the tool pickup 
coils detect near fields; hence, the lead frames (because of their closer 
proximity to the pickup coils) indicate a disproportionately high field level 
relative to any PCB surface (microstrip) traces. The field strength is 
comprised of 
first-order, second-order, and third-order rolloff terms. Therefore, the field 
signature would show much less relative differences (even with very small 
spacing displacements) because of an exponential rolloff in the coupled signal; 
hence, some test results may be misleading. Please be aware that I am in 
agreement with you on the benefits of low-profile lead packages. Any 
should measure the fields from a small daughter board connected via standoffs 
1/4 to 3/8 inch length, as the results will scare you.

Re: your statement, "None of the papers did such an experiment in a way that 
could be used to bet money on." 

As (many months) before, I disagree. I demonstrated the relative radiation 
and crosstalk performance of microstrip (50 & 100 Ohm lines), guarded 
(50 Ohms), stripline (50 Ohms), and guarded stripline (50 Ohms) as part of 
the (now ancient) Hewlett-Packard High-Speed Digital Design Seminar Series 
included such respected pros as Ed Sayre, Eric Bogatin, and Henri Merkelo). 
The results were clear that either containment (via an enclosure) or the use of 
stripline was needed for FCC or CISPR Class B compliance. The data and 
knowledge gained from these findings led to the redesign of scores (yes, 
of EMI-deficient PCBs over the following decade that achieved a typical 20 dB 
(some as high as 40 dB) reductions in radiated emissions. No one has yet to 
find that the HP spectrum analyzers, HP near-field probes, EMCO (far-field) 
antennas and near-field probes that I used (and still use) were technically 
deficient in any way. Additionally, my software predictions support the 
test data as well.

My concern (and the only reason I'm sending these comments) is that less 
experienced designers than yourself will think surface traces are "no problem" 
NOT employ the many other routing techniques that you and I have learned over 
the years to be beneficial (or mandatory) for a successful design. Obviously, 
non-enclosed/shielded designs will suffer most from this oversight.

Good engineering to all,


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:

For help:
si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field

List technical documents are available at:

List archives are viewable at:     
or at our remote archives:
Old (prior to June 6, 2001) list archives are viewable at:

Other related posts: