[SI-LIST] Re: Traces don't cause EMI - really?
- From: steve weir <weirsp@xxxxxxxxxx>
- To: MikonCons@xxxxxxx, leeritchey@xxxxxxxxxxxxx
- Date: Mon, 02 Feb 2004 04:43:33 -0800
Mike, I think the issue is worth reviewing under current
circumstances. Some understandings have improved greatly with regard to
antenna design and/or detuning, and geometries have definitely changed for
the better. Lee advocates a buried microstrip for the outermost routing
layer. That captures the vast majority of the field in the dielectric.
It's been a long time since I read those old papers going back to the mid
eighties when stripline started getting promoted for EMI. But I am
confident that we will find all of those studies compared surface
microstrip to stripline. It would be interesting to repeat your 50 ohm
tests with this "buried microstrip" versus a true surface microstrip for EMI.
Regards,
Steve
At 03:30 PM 2/1/2004 -0500, MikonCons@xxxxxxx wrote:
>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. As
>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
>disbeliever
>should measure the fields from a small daughter board connected via
>standoffs of
>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
>microstrip
>(50 Ohms), stripline (50 Ohms), and guarded stripline (50 Ohms) as part of
>the (now ancient) Hewlett-Packard High-Speed Digital Design Seminar Series
>(that
>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,
>hundreds)
>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
>empirical
>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" and
>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,
>
>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 technical documents are available at:
> http://www.si-list.org
>
>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 technical documents are available at:
http://www.si-list.org
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:
