From: Lee Ritchey ([email protected])
Date: Mon Dec 27 1999 - 16:39:55 PST
I'm aware of such measurements. This does not answer my question, which
was, is this radiation loss significant in terms of EMI? Lots of EMI
measurements day it is not.
To suggest that I dismissed these losses is to put words in my nouth
that I did not say. Reread my previous reply.
To suggest that we should be concerned about these losses without first
quantifying them and determining that they are significant in the
context of the question is what is near sighted.
Lee
Ron Miller wrote:
> Lee
>
> The microwave guys IEEE MTT Society have been making measurements of
> radiation from pcbs on microstrip since the 50s.
>
> They normally catagorize RF losses in order of importance into:
> 1. Dielectric losses
> 2 . Scin effect and resistive losses
> 3. Radiation losses.
>
> Since radiation is considered a loss by this community, it seems
> rather near-sighted
> to dismiss it for uninterupted traces across uninterupted planes.
> Obviously, the problem
> is agrivated at every discontinuity in impedance causing reflections
> and circulating
> currents.
>
> Ron Miller
>
> Lee Ritchey wrote:
>
>> Throughout these discussion I see words like "substantial",
>> "significant", etc. suggesting that these problems are big enough to
>> worry about. Have any of
>> you made real measurements to quantify the problem? Are we worrying
>> about something that is in the noise? My experience and many
>> measurements show that
>> traces running along the surface of a multilayer PCB with
>> uninterupted planes do not cause measurable EMI. Doug Brooks and
>> the UMR people even did a set
>> of tests to verify this and published a report in PC Design.
>>
>> By uninterupted I mean without isolation cuts. The normal holes in
>> planes needed to accommodate vias are not problems unless they
>> overlap and make slits.
>>
>> sweir wrote:
>>
>> > Jian,
>> >
>> > The assumption which I have made is that we have a multilayer
>> board in both
>> > cases. So, in the microstrip case, we still have the problem that
>> when we
>> > via, we leave the TEM mode as well. Without a matching via
>> between the two
>> > ground planes, we cause considerable excitation in both:
>> >
>> > ====| S
>> > =============== G
>> > |
>> > ========|====== G
>> > |==== S
>> >
>> > For this situation, I do not see that the stripline is
>> fundamentally better
>> > or worse as the planes in both cases are subjected to substantial
>> > pertubations. Do you agree that if we want to keep the EMI down,
>> we want
>> > to stay in TEM as much as possible? My understanding of the world
>> is that
>> > this means we can't let the field expand substantially into
>> > dielectric. So, we need a Z axis return path to mirror the Z axis
>> signal
>> > path as closely as possible.
>> >
>> > If I am way off base, I welcome the education.
>> >
>> > Regards,
>> >
>> > Steve.
>> >
>> > At 03:01 PM 12/21/99 -0800, you wrote:
>> > >Hi, Steve:
>> > >
>> > >I am not sure what "reflection plane to reflection plane vias"
>> mean in your
>> > >message. Maybe it is defined earlier in this subject. I did not
>> get all the
>> > >messages on this subject because my name was removed accidentally
>> from the
>> > >SI-LIST due to a crash on the SI-LIST server. My last posted
>> message is
>> > >mainly an objection to the comment "stripline normally radiates
>> more".
>> > >Basically, this comment is normally true. However, there are
>> exceptions.
>> > >
>> > >Regarding vias on microstrip circuits mentioned in your posting,
>> the
>> > >purposes for the vias in microstrip circuits may be different
>> from that for
>> > >stripline circuit:
>> > >
>> > >A microstrip line has two metals: one for the strip and the other
>> for the
>> > >ground. There exist only one TEM or quasi-TEM mode on a
>> microstrip circuit.
>> > >
>> > >An illustration on microstrip
>> > > ===== strip
>> > >
>> > >============== ground
>> > >
>> > >A stripline circuit has three metals: (1) the strip; (2) the top
>> ground
>> > >plane; (3) the bottom ground plane. We can excite a TEM or
>> quasi-TEM mode
>> > >between any two metals. However, we normally use the mode with
>> the excited
>> > >between the strip (+ terminal) and the two ground planes (-
>> terminals). Any
>> > >3D interconnects or holes on the ground planes may excite the
>> parallel plate
>> > >mode. The parallel plate mode is between the two ground planes.
>> One of the
>> > >ground planes becomes the positive terminal and the other become
>> negative.
>> > >The parallel plate mode can be surpressed by building a via to
>> connect the
>> > >top and bottom ground plane at the proximity of the vertical 3D
>> > >interconnect. It is very effective.
>> > >
>> > >
>> > >An illustration on strip line.
>> > >
>> > > ================ top ground
>> > > === strip
>> > > ================ bottom ground
>> > >
>> > >For microstrip structure, there is no parallel plate mode and we
>> do not need
>> > >to use vias to surpress them. However, some people do try to use
>> vias to
>> > >suppress the surface wave mode, which is normally much less
>> serious than the
>> > >parallel plate mode in stripline circuits. However, it is not
>> very
>> > >effective. In this sense, the vias in microstrip circuits and
>> strip line
>> > >circuits should serve different purposes. Thank you very much.
>> > >
>> > >Best regards,
>> > >
>> >
>> >----------------------------------------------------------------------------
>>
>> > >------------
>> > >Jian-X. Zheng, Ph.D
>> > >Zeland Software, Inc., 39676 Mission Blvd., Fremont, CA 94539,
>> U.S.A.
>> > >Tel: 510-797-8109, Fax: 510-797-8241, Web: http://www.zeland.com
>> >
>> >----------------------------------------------------------------------------
>>
>> > >------------
>> > > > -----Original Message-----
>> > > > From: [email protected]
>> > > > [mailto:[email protected]]On Behalf Of sweir
>> > > > Sent: Tuesday, December 21, 1999 11:19 AM
>> > > > To: [email protected]
>> > > > Subject: RE: [SI-LIST] : Inner vs. Outer Layer Routing
>> > > >
>> > > >
>> > > > Jian,
>> > > >
>> > > > I believe that the need for reflection plane to reflection
>> plane vias
>> > > > proximate to high speed signal vias is the same for microstrip
>> as
>> > > > it is for
>> > > > stripline.
>> > > >
>> > > > Regards,
>> > > >
>> > > >
>> > > > Steve.
>> > > >
>> > > > At 12:57 PM 12/21/99 -0800, you wrote:
>> > > > >Hi, everybody:
>> > > > >
>> > > > >Microstrip and stripline have their own advantage. Stripline
>> normally has
>> > > > >less inductance and less dispersion. However, 3D interconnect
>> in
>> > > > stripline
>> > > > >may create very strong radiation. Some person mentioned that
>> stripline
>> > > > >radiates less. Such a conclusion is true when you have only
>> the
>> > > > horizontal
>> > > > >straight lines or horizontal bends. However, if you have
>> vertical
>> > > > >interconnects in a stripline circuit, the vertical
>> interconnects
>> > > > may create
>> > > > >very strong radiation. It is the so-called parallel plate
>> mode, and this
>> > > > >mode does not have any cut off frequency. Normally, microwave
>>
>> > > > designers use
>> > > > >shorting pin between the two ground planes at the proximity
>> of 3D
>> > > > >interconnects to suppress the parallel plate mode. Thanks!
>> > > > >
>> > > > >Best regards,
>> > > > >
>> > > >
>> >-----------------------------------------------------------------
>> > > > -----------
>> > > > >------------
>> > > > >Jian-X. Zheng, Ph.D
>> > > > >Zeland Software, Inc., 39676 Mission Blvd., Fremont, CA
>> 94539, U.S.A.
>> > > > >Tel: 510-797-8109, Fax: 510-797-8241, Web:
>> http://www.zeland.com
>> > > >
>> >-----------------------------------------------------------------
>> > > > -----------
>> > > > >------------
>> > > > > >
>> > > > >
>> > > > >
>> > > > >**** To unsubscribe from si-list: send e-mail to
>> > > > >[email protected]. In the BODY of message put:
>> UNSUBSCRIBE
>> > > > >si-list, for more help, put HELP.
>> > > > >si-list archives are accessible at
>> http://www.qsl.net/wb6tpu/si-list
>> > > > >****
>> > > >
>> > > >
>> > > > **** To unsubscribe from si-list: send e-mail to
>> > > > [email protected]. In the BODY of message put:
>> > > > UNSUBSCRIBE si-list, for more help, put HELP.
>> > > > si-list archives are accessible at
>> http://www.qsl.net/wb6tpu/si-list
>> > > > ****
>> > > >
>> > > >
>> > >
>> > >
>> > >**** To unsubscribe from si-list: send e-mail to
>> > >[email protected]. In the BODY of message put:
>> UNSUBSCRIBE
>> > >si-list, for more help, put HELP.
>> > >si-list archives are accessible at
>> http://www.qsl.net/wb6tpu/si-list
>> > >****
>> >
>> > **** To unsubscribe from si-list: send e-mail to
>> [email protected]. In the BODY of message put: UNSUBSCRIBE
>> si-list, for more help, put HELP.
>> > si-list archives are accessible at
>> http://www.qsl.net/wb6tpu/si-list
>> > ****
>>
>> **** To unsubscribe from si-list: send e-mail to
>> [email protected]. In the BODY of message put: UNSUBSCRIBE
>> si-list, for more help, put HELP.
>> si-list archives are accessible at
>> http://www.qsl.net/wb6tpu/si-list
>> ****
>
> --
> Ronald B. Miller _\\|//_ Signal Integrity Engineer
> (408)487-8017 (' 0-0 ') fax(408)487-8017
> ==========0000-(_)0000===========
> Brocade Communications Systems, 1901 Guadalupe Parkway, San Jose, CA 95131
> [email protected], [email protected]
>
>
**** To unsubscribe from si-list: send e-mail to [email protected]. In the BODY of message put: UNSUBSCRIBE si-list, for more help, put HELP.
si-list archives are accessible at http://www.qsl.net/wb6tpu/si-list
****
This archive was generated by hypermail 2b29 : Tue Feb 29 2000 - 11:39:15 PST