Thanks for that Lee!
I've read a lot about using spread weave (I've also watched a Lee youtube
video) although I've not found anything specifically about using 2-ply of
spread weave glass. Were I can find more information about that?
Regards,
Eduardo.
-----Mensagem original-----
De: Lee Ritchey [mailto:leeritchey@xxxxxxxxxxxxx] ;
Enviada em: segunda-feira, 6 de junho de 2016 15:10
Para: 'Ken Cantrell' <ken@xxxxxxxxxxxxxxxx>; scott@xxxxxxxxxxxxx;
endler@xxxxxxxxxxxxxx
Cc: si-list@xxxxxxxxxxxxx
Assunto: RE: [SI-LIST] Re: RES: Re: ??: Re: Variation of PCB Dielectric
Properties
Actually, this info was not free! We spend $100K plus on test vehicles to get
it. Most don't have the resources to do that, so we chose to share the results.
-----Original Message-----
From: Ken Cantrell [mailto:ken@xxxxxxxxxxxxxxxx]
Sent: Monday, June 6, 2016 10:24 AM
To: scott@xxxxxxxxxxxxx; endler@xxxxxxxxxxxxxx
Cc: Lee Ritchey <leeritchey@xxxxxxxxxxxxx>; si-list@xxxxxxxxxxxxx
Subject: RE: [SI-LIST] Re: RES: Re: ??: Re: Variation of PCB Dielectric
Properties
All -
I think 2-ply each side is generic now. Accepted practice. Of course I stole
it Scott/Yuri/Lee et. al. I read their stuff:) And it's free!
Ken
-----Original Message-----
From: [mailto:si-list-bounce@xxxxxxxxxxxxx] On Behalf Of Scott McMorrow
Sent: Monday, June 06, 2016 10:42 AM
To: endler@xxxxxxxxxxxxxx
Cc: Lee Ritchey <leeritchey@xxxxxxxxxxxxx>; si-list@xxxxxxxxxxxxx
Subject: [SI-LIST] Re: RES: Re: ??: Re: Variation of PCB Dielectric Properties
he uses 2-ply on each side of the stripline, just as I do.
Scott McMorrow
R&D Consultant
Teraspeed Consulting - A Division of Samtec
16 Stormy Brook Rd
Falmouth, ME 04105
(401) 284-1827 Business
http://www.teraspeed.com
On Mon, Jun 6, 2016 at 12:29 PM, DATACOM - Endler <endler@xxxxxxxxxxxxxx>
wrote:
Lee,
By using two plies of mechanically spread glass you mean using 2-ply
laminates on each side of the stripline, right? Or it's 1-ply on each side?
Regards,
Eduardo.
-----Mensagem original-----
De: si-list-bounce@xxxxxxxxxxxxx [mailto:si-list-bounce@xxxxxxxxxxxxx]
Em nome de Lee Ritchey Enviada em: quarta-feira, 1 de junho de 2016
19:08
Para: dmarc-noreply@xxxxxxxxxxxxx; shlepnev@xxxxxxxxxxxxx; 'Jeff Loyer'
<jeff.loyer@xxxxxxxxxx>
Cc: si-list@xxxxxxxxxxxxx
Assunto: [SI-LIST] Re: ??: Re: Variation of PCB Dielectric Properties
In our DesignCon paper in 2013 we showed that the difference between
HVLP copper and reverse treat had the effect of increasing the DK
slightly. We surmise that this is due to a very small increase in
effective capacitance due to the higher profile of the reverse treat copper.
On the weave effect front, we get around all of the issues I have seen
discussed here by using two plies of mechanically spread glass. Doing
this, we have seen no more than 2 pS skew on any of our 19G links of
which there are about 200 on the latest design.
-----Original Message-----
From: si-list-bounce@xxxxxxxxxxxxx
[mailto:si-list-bounce@xxxxxxxxxxxxx]
On
Behalf Of Bert Simonovich (Redacted sender "bertsimonovich" for DMARC)
Sent: Wednesday, June 1, 2016 2:32 PM
To: shlepnev@xxxxxxxxxxxxx; 'Jeff Loyer' <jeff.loyer@xxxxxxxxxx>
Cc: si-list@xxxxxxxxxxxxx
Subject: [SI-LIST] Re: ??: Re: Variation of PCB Dielectric Properties
Yuriy,
How do you factor in phase delay due to copper roughness? Most field
solvers do not have this capability either. It has been shown in
various papers that roughness adds additional phase delay. If
roughness is not accounted for, then that too can account for
variation in Dk between manufacturers' data and measured results.
Bert Simonovich
Signal/Power Integrity Practitioner | Backplane Specialist | Founder
LAMSIM Enterprises Inc.
Web Site: http://lamsimenterprises.com
Blog: http://blog.lamsimenterprises.com/
-----Original Message-----
From: si-list-bounce@xxxxxxxxxxxxx
[mailto:si-list-bounce@xxxxxxxxxxxxx]
On
Behalf Of Yuriy Shlepnev
Sent: 1-Jun-16 1:25 PM
To: 'Jeff Loyer'
Cc: si-list@xxxxxxxxxxxxx
Subject: [SI-LIST] Re: ??: Re: Variation of PCB Dielectric Properties
Jeff,
As I mentioned, it is all about the homogenization scale, comparing to
the cross-section.
One dielectric model can be used for loosely coupled traces for
instance with small difference in the velocity or delay of odd and
even mode (no FEXT).
On the other hand, when you see larger difference in the propagation
velocity or delay of two modes (larger FEXT), two-dielectric model is
needed.
Correlating just differential impedance and insertion loss does not
provide a complete solution if you want to use such model in a link path
analysis.
See more details and practical examples of model building at our
DesignCon "Lessons learned..." paper #2014_01 at
http://www.simberian.com/AppNotes.php
Slides 19 and 22,23 in particular illustrate the need of
two-dielectric model - the FEXT level or modal phase delay can be used
to make such decision.
Best regards,
Yuriy
Yuriy Shlepnev, Ph.D.
President, Simberian Inc.
2629 Townsgate Rd., Suite #235, Westlake Village, CA 91361, USA Office
+1-702-876-2882; Fax +1-702-482-7903 Cell +1-206-409-2368; Virtual
+1-408-627-7706
Skype: shlepnev
www.simberian.com
Simbeor – Accurate, Productive and Cost-Effective Electromagnetic
Signal Integrity Software 2010 and 2011 DesignVision Award Winner,
2015 Best In Design&Test Finalist
-----Original Message-----
From: Jeff Loyer [mailto:jeff.loyer@xxxxxxxxxx]
Sent: Wednesday, June 1, 2016 10:04 AM
To: shlepnev@xxxxxxxxxxxxx
Cc: si-list@xxxxxxxxxxxxx
Subject: RE: [SI-LIST] ??: Re: Variation of PCB Dielectric Properties
Hello Yuriy,
Could you clarify when you need to include the resin layer? In the
work I've seen, it hasn't been necessary to include the resin layer to
correlate differential impedance or insertion loss results, but can
affect FEXT significantly (see DesignCon 2015 paper " PCB Material and
Copper Foil Considerations for Insertion Loss"). Is there a
particular frequency or modeling instance where neglecting the resin
layer causes large modeling errors (compared to measurements).
I.E., when do I need to add the complexity of properly modeling the
resin layer in my simulations, and when can it be neglected?
Thanks,
Jeff Loyer
-----Original Message-----
From: Yuriy Shlepnev [mailto:shlepnev@xxxxxxxxxxxxx]
Sent: Wednesday, June 1, 2016 9:55 AM
To: pcb_layup@xxxxxxx; jeff.loyer@xxxxxxxxxx;
richard.allred@xxxxxxxxx; 'Istvan Novak'
Cc: dmarc-noreply@xxxxxxxxxxxxx; si-list@xxxxxxxxxxxxx
Subject: RE: [SI-LIST] ??: Re: Variation of PCB Dielectric Properties
Terry,
Good points, especially #6 - " accurate filed solver with resin-filled
layer model is necessary " :-)
There are 3 key elements in the broadband material model
identification with t-lines (identification with GMS-parameters or
with IPC's SPP
technique):
1) High quality measurements;
2) Use of actual geometry of the t-line cross-section;
3) Accurate field solver with proper material and dielectric
inhomogeneity modeling; This is assuming that the test fixtures are
properly designed and manufactured (something like in SPP standard or
on Wild River Technology validation platforms).
Missing one of those key elements will give you the Dk or Df numbers
that are substantially off from the dielectric manufacturer's data.
The big discrepancy, as you observed below, should be actually the
first sign that something is wrong with the procedure or you are
dealing with the structures that requires homogenization approach
other than used by the laminate manufacturer.
As Scott mentioned, the spreadsheet data are usually not so bad. Some
manufacturers, Isola for instance, have accurate Dk values measured
for the Z-direction (wide strip line resonator or Berezkin's method).
In the projects with the Isola's materials we usually end up with just
2-3% adjustment of Dk for single-ended strips or microstrips (slightly
larger Dk due to presence of the X and Y-components of the electric
field in narrower lines). Same is valid for Meg6 and some other
materials from manufacturers with the established characterization
process. The smaller the X and Y components of the electric field of a
line, the closer you should get to the spreadsheet values of Dk at the
specified frequency. It is all about the homogenization and scale -
see more at our DesignCon tutorial -#2016_01 at
http://www.simberian.com/TechnicalPresentations.php
Following the homogenization scale approach, we can conclude that the
inhomogeneous dielectric cannot be uniquely homogenized for the cases
of tightly coupled strip or microstrip differential lines. To have
correlation in the impedance and propagation constant for both
differential and common modes you will need a model with at least two
dielectrics - resin or solder mask and the homogenized mixture. When
model for resin is not available (those are proprietary mixtures :-),
you can derive it from the glass model (you can get this data from the
fabric
manufacturers) and volumetric resin content as it is done in our paper
#2014_04 at http://www.simberian.com/AppNotes.php.
Best regards,
Yuriy
Yuriy Shlepnev, Ph.D.
President, Simberian Inc.
2629 Townsgate Rd., Suite #235, Westlake Village, CA 91361, USA Office
+1-702-876-2882; Fax +1-702-482-7903 Cell +1-206-409-2368; Virtual
+1-408-627-7706
Skype: shlepnev
www.simberian.com
Simbeor C Accurate, Productive and Cost-Effective Electromagnetic
Signal Integrity Software
2010 and 2011 DesignVision Award Winner, 2015 Best In Design&Test
Finalist
-----Original Message-----
From: si-list-bounce@xxxxxxxxxxxxx
[mailto:si-list-bounce@xxxxxxxxxxxxx]
On
Behalf Of SI List
Sent: Tuesday, May 31, 2016 9:47 AM
To: jeff.loyer@xxxxxxxxxx; richard.allred@xxxxxxxxx; 'Istvan Novak'
Cc: dmarc-noreply@xxxxxxxxxxxxx; si-list@xxxxxxxxxxxxx
Subject: [SI-LIST] ??: Re: Variation of PCB Dielectric Properties
Hello:
Sharing some data and my experience from the view of PCB maker for
reference.
1. There is a gap between measured and simulated impedance, Especially
on differential stripline. The measured impedance will be bigger than
simulated impedance 3%~10%<Normal Dk ~Very Low DK> ). So PCB maker
need to tweak trace width/space. PCB maker will use real cross-section
geometry parameters to back-calculate the DK, and setup a modified
material DK database.
2. Back-calculated DK varied from cross-section geometry; single-end
or differential model; prepreg combination etc. We ever did over 500
micro-sections from dedicated standard impedance coupons for Dk
back-calculate analysis. But we confused when we tried to fixed a
back-calculated DK for a material to guide impedance design.
Base Material PP
Style CITS25 SI8000 Datasheet Variation
Isola-FR408 1080
RC63% 3.08 3.12 3.51 0.39
Isola-FR408 2116
RC53% 3.12 3.13 3.73 0.6
Isola-IS415 1080
RC65% 3.05 3.02 3.52 0.5
Isola-IS415 2116
RC55% 3.06 3.08 3.72 0.64
TUC-TU862 1080
RC67% 3.4 3.43 4.1 0.67
TUC-TU862 2116
RC56% 3.63 3.6 4.3 0.7
TUC-TU862 2116
RC60% 3.8 3.81 4.3 0.49
EMC-EM370D 1080
RC63% 3.24 3.28 3.8 0.52
EMC-EM370D 2116
RC52% 3.47 3.44 4.1 0.66
EMC-EM370D 7629
RC44% 3.66 3.7 4.2 0.5
ITEQ-IT200LK 1080
RC65% 3.14 3.15 3.68 0.53
ITEQ-IT200LK 2116
RC57% 3.14 3.13 3.83 0.7
ITEQ-IT200LK 7628
RC50% 3.31 3.3 3.99 0.69
3. Single-end stripline is more sensitive on Z-axis DK, differential
stripline is more sensitive on X-Y axis DK. So Pure resin filled layer
and buttercoat layer will be the key factors to an accurate
differential stripline simulation. But there 2 limitations, A: how to
get DK of pure resin; B: Resin filled differential stripline model
seems inaccurate (now PCB maker used field solver).
4. FR4 glass-resin Mixed dielectric lead to the gap between measured
and simulated impedance. Rotate the layout with 5~15 degree angel will
migrate FWE (I think the impedance wave will more stable), but can not
eliminate the gap.
5. The back-calculated DK used by PCB maker setup a barrier. Layout
cannot communicate easily with fab house on stackup impedance design. Generic
vs.
specific stackups is still a problem. If the DK from datasheet can be
used and useful downstream, the barrier will disappear.
6. DK is not constant, vary from Prepreg combination, copper weight,
copper remain ratio and Z-axis or X-Y axis etc. So the best way to
improve simulation accuracy is the DK simulation technology on a specific
stackup.
The key points is get the mixed DK of prepreg combination after
lamination resin flowed and the DK of pure resin. Also accurate filed
solver with resin-filled layer model is necessary.
Reference paper:
Designcon 2013: ACCURATE INSERTION LOSS AND IMPEDANCE MODELING OF PCB
TRACES
Best regards,
Terry Ho
www.sisolver.com
-----邮件原件-----
å‘件人: si-list-bounce@xxxxxxxxxxxxx
[mailto:si-list-bounce@xxxxxxxxxxxxx]
代衚 Jeff Loyer
å‘é€æ—¶é—Ž: 2016幎5月31æ—¥ 22:32
收件人: richard.allred@xxxxxxxxx; Istvan Novak
抄é€: dmarc-noreply@xxxxxxxxxxxxx; si-list@xxxxxxxxxxxxx
䞻题: [SI-LIST] Re: Variation of PCB Dielectric Properties
Hi Richard,
When I was with Intel I was heavily involved in this topic and I
believe our Fiber Weave Effect: Practical Impact Analysis and
Mitigation Strategies ?paper contains a synopsis of the data
available. In it we analyzed the raw data from the work done by the
Intel DDR folks to try to glean the type of statistical data you re
after ?the net effect of the fiberglass weave on propagation delay.
I ve attached a snapshot from that paper (sorry, others won t be
able to see it) showing the distribution of the raw data. Bert
Simonovich did some work to prove that it can be replicated in
simulation, see http://lamsimenterprises.com/.
To my knowledge, no one has performed further studies ?it was a
unique, wonderful intersection of energies and funds that allowed this
study to be done since it involved so many different material and PCB
vendors across the world.
Jeff Loyer
Signal and Power Integrity Product Manager
Altium US, www.altium.com
4225 Executive Square, Suite 700
La Jolla, CA 92037
360-819-2520 (cell)
858-864-1580 (desk)
-----Original Message-----
From: si-list-bounce@xxxxxxxxxxxxx
[mailto:si-list-bounce@xxxxxxxxxxxxx]
On
Behalf Of Richard Allred
Sent: Tuesday, May 31, 2016 5:45 AM
To: Istvan Novak
Cc: dmarc-noreply@xxxxxxxxxxxxx; si-list@xxxxxxxxxxxxx
Subject: [SI-LIST] Re: Variation of PCB Dielectric Properties
Thanks for the comments, they helped me clarify my thoughts.
As you guessed, I am interested in finding the statistical
distribution of the dielectric "constant" property across high volume
manufacturing so I can understand how the absolute delay of the line
varies. Determining the output statistical variation of a system,
given the input variable distribution, is one of my current pet
projects.
I was able to find a very interesting presentation by Gary Brist of
Intel (from the early 2000's) where he discusses in extreme detail the
manufacturing process variation for FR4. Slide # 91, 97 and 106
contained the e_r information was was after.
https://www.jlab.org/eng/eecad/pdf/053designop.pdf
The bottom line is that e_r varies due to the resin content and the
spatial proximity of the copper trace to the glass bundle (weave
effect). My guess is that if there is an updated study on current
materials for high speed PCB that it is likely proprietary.
Regards,
Richard Allred
On Tue, May 31, 2016 at 6:02 AM, Istvan Novak
<istvan.novak@xxxxxxxxxxx>
wrote:
Vadim,
I agree with what you say. In this particular case though the
question came from someone working for an EDA company, making it
much
less likely that they can affor or want to go into the business of
designing/evaluating printed circuit boards themselves. Until we
get
to a point that the glass and resin electrical properties differ
much
less and they are described in more detail on the data sheet, this
question will remain just partially answered. Though to the credit
of
laminate and pcb vendors, they have come a long way to supply more
data. A lot is already posted available for everyone and even moreavailable with nondisclosure agreements.
is
Regards,
Istvan Novak
Oracle
On 5/31/2016 3:46 AM, heyfitch (Redacted sender heyfitch for DMARC)wrote:
Hi Richard -
I may not exactly be answering your question here.....
The more you specify to a fab house the less you leave to chance.
You can pick a specific dielectric from a menu of offerings with a
thickness"known thickness and a RC (resin content). The so called "pressed
out
would depend on the % of copper fill. The default number is usually
given for 50%, but you can ask a fab for the number for your design
the target Z.before you give'em a go. The trace width is what a fab adjusts to
hit
They don't tweak RC for this purpose. Higher RC dielectric usually
has lower Dk and higher Df. Some dielectric vendors show
explicitly
in their datasheets the Dk values for each available option of RC.
(RTF, VLP, HVLP).The effective Df is very strongly affected by the choice of copper
foil
That is if you roll the loss due to copper surface roughness into
the
dielectric's Df parameter. It's not necessary to do so if you have
built enough many coupons to unambiguously separate Df and copper
surface roughness parameters in you simulation model (by way
of deembeding generalized model s-parameters.)
This is all good but here comes a reality check...
I have seen internal data from a reputable fab of their own
impedance
coupon measurement. To my surprise, the impedance values were
distributed almost uniformly between -10% and +10% of the target.
They did not show any outliers, which made me think the fab used
this
coupon measurement - one per panel - for sorting.
With such a uniform distribution their yield must have been quite low.
(For microstrips, the actual Z is also affected by the amount of
over-plating and the solder mask, changing it by up to 3-4 Ohms.).
To muddy up this already confusing picture, one should consider how
fabs use Polar Instrument HW and SW - the de-facto standard with
them
error.- to determine impedance of a panel coupon, which leads to a
systematic
But that is a whole other can of worms that I will not get into here.
My recommendation, if you asked for one, is to include you own
connectorized coupons in your design, and measure them; then fit
GMS-parameters with the model. And, yes, "waste" space on the panel
for the coupons; this will make you many friends among project
managers left and right. ;). But, in the end, you will know
exactly
the impedance, the dielectric, and surface roughness model
parameters. If you stay with the same fab thru many designs - and
this fab is.avoid fab brokers - you may even collect useful data on how
consistent
Best regards,
Vadim Heyfitch
Sent from my phone
On May 29, 2016, at 6:03, Richard Allred <richard.allred@xxxxxxxxx>
wrote:
Greetings,
I am aware that typical PCB manufacturers usually guarantee some
impedance target (+/- 10 or 15%) for high speed traces and that
they
may use any number of manufacturing controls to achieve this. The
result is that the only way to know the geometric dimensions of a
given sample is to cross-section it.
What I am interested in is, what kind of variation can be expected
in
the effective dielectric properties due to the PCB manufacturers
tweaking of the glass/resin ratio and the geometrical variation?
Is
anyone aware of a published study that reports this?
Kind regards,
Richard Allred
www.SiSoft.com
------------------------------------------------------------------
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 forum is accessible at:
http://tech.groups.yahoo.com/group/si-list
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
------------------------------------------------------------------
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 forum is accessible at:
http://tech.groups.yahoo.com/group/si-list
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
------------------------------------------------------------------
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 forum is accessible at:
http://tech.groups.yahoo.com/group/si-list
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
------------------------------------------------------------------
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 forum is accessible at:
http://tech.groups.yahoo.com/group/si-list
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
------------------------------------------------------------------
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 forum is accessible at:
http://tech.groups.yahoo.com/group/si-list
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
------------------------------------------------------------------
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 forum is accessible at:
http://tech.groups.yahoo.com/group/si-list
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
-----
No virus found in this message.
Checked by AVG - www.avg.com
Version: 2016.0.7598 / Virus Database: 4591/12335 - Release Date:
05/31/16
------------------------------------------------------------------
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 forum is accessible at:
http://tech.groups.yahoo.com/group/si-list
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
------------------------------------------------------------------
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 forum is accessible at:
http://tech.groups.yahoo.com/group/si-list
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
------------------------------------------------------------------
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 forum is accessible at:
http://tech.groups.yahoo.com/group/si-list
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
