[SI-LIST] Re: AW: Re: Some reference on reference planes
- From: steve weir <weirsi@xxxxxxxxxx>
- To: si-list@xxxxxxxxxxxxx
- Date: Mon, 14 Nov 2011 09:00:55 -0800
Larry, Jory, it all depends of course. And in that I advocate doing the
homework.
Thin dielectric does a better job suppressing resonant peaks than does
thick dielectric with equivalent loss tangent. As shown in several
papers including one that Istvan's group presented several years ago,
the smaller that we make cavity polygons, the higher their Q. If we do
the homework we can figure out whether our best choice is in terms of
stack-up and routing that will get us reliably to our performance goals
with the least cost and grief.
Best Regards,
Steve.
On 11/14/2011 8:28 AM, Smith, Larry wrote:
> Jory - your point is well taken. Thin power plane dielectric does not
> guarantee low PDN impedance because cavity resonance may exist which raises
> up impedance peaks at some frequencies. I think we can say that the PDN will
> not be low impedance at high frequency if the dielectric is thick (power
> plane is several stackup positions away from ground plane). Your examples
> demonstrate how even thin power plane dielectrics will have impedance peaks.
> This may create problems for both the signal integrity on the traces and the
> power integrity for the victim PDN.
> The safest thing to do is simply avoid running signal traces over return
> plane splits. If you do cross splits, the damage done is proportional to the
> number of offending traces and their probability of switching at the same
> time. This can be mitigated somewhat by using differential signals, but as
> Scott clearly articulated, there can be trouble here also (EMI). Even if the
> signals are perfectly differential at the driver, skew develops if the
> differential traces are slightly different lengths, and that can be enough to
> stimulate plane resonances.
>
> It seems that many signal and power integrity issues boil down to how well
> you handle the return path. For economic reasons, our industry often cheats
> on the return path and tries to live with the consequences.
>
> Regards,
> Larry Smith
> Qualcomm
>
> From: Jory McKinley [mailto:jory_mckinley@xxxxxxxxx]
> Sent: Saturday, November 12, 2011 11:50 AM
> To: Smith, Larry; Lee Ritchey; Mark Grobman; Havermann, Gert
> Cc: si-list@xxxxxxxxxxxxx
> Subject: Re: [SI-LIST] Re: AW: Re: Some reference on reference planes
>
> Larry and List,
>
> "In the GHz band, the impedance of the PDS will be low as long as the
> dielectric thickness from power to ground plane is small"
>
> This can be tricky, as you know the PDN impedance cannot be controlled above
> a couple hundred Mhz on a PCB and the signal Via's (that are not stitched
> correctly) that cross these PDN cavities may excite natural resonances that
> occur due to shape. PCB planar capacitance may shift the resonances but will
> not remove them. This holds for package PDN except the interaction of PCB
> and package PDN create a series of parallel and series resonances at higher
> frequencies.
>
> We worked on project very recently (I can share the real data in the near
> future) where a customer was getting very poor jitter lab measurements on
> multiple chip PLL's and not meeting PCIe gen3 specs. We found that the chip
> package PLL power plane had a few high speed signals past through the
> z-direction with poor via stitch return. We determined that the PLL power
> plane had resonances that could be excited by the frequency content on the
> high speed signals. There where other issues with the package design
> (unrelated) as well so we recommended a new package design that reduced the
> shape of the PLL power plane and re-routed the high speed signals. Package
> re-design came back and the jitter numbers improved to a point of passing
> compliance.
>
> Regards,
> -Jory
>
>
>
> ________________________________
> From: "Smith, Larry"<larrys@xxxxxxxxxxxx>
> To: Lee Ritchey<leeritchey@xxxxxxxxxxxxx>; Mark
> Grobman<markgrobman@xxxxxxxxx>; "Havermann, Gert"<Gert.Havermann@xxxxxxxxxxx>
> Cc: "si-list@xxxxxxxxxxxxx"<si-list@xxxxxxxxxxxxx>
> Sent: Wednesday, November 9, 2011 5:28 PM
> Subject: [SI-LIST] Re: AW: Re: Some reference on reference planes
>
> Lee and all - You have some good comments in your response but I feel we are
> missing some important concepts in this thread. How many signals are going
> to cross the plane cut on this high performance PCB? If it is just one, the
> consequences will be minimal. If it is 100 - watch out!
>
> We know what happens to the current on the 50 Ohm trace that crosses the
> plane cut, it just goes straight across while it suffers from a small
> impedance discontinuity. But what happens to the return current? The answer
> depends upon the frequency band where we ask the question. As several
> posters on this thread have pointed out, a fast rise time signal will have
> GHz frequency content and the return current in that frequency band must make
> its way across the plane split through each power plane capacitance to
> (hopefully continuous) ground plane somewhere in the stackup. If the signal
> pulse has a long duration and is parallel terminated at the far end, return
> current at 100's and 10's of MHz will find its way through discrete ceramic
> and bulk decoupling capacitors. If the signal pulse lasts for a very long
> time, return current in the kHz band down to DC will return through the
> voltage regulator.
>
> When the signal edge hits the plane discontinuity, power plane bounce ripples
> out in space with the disturbance uncovering more and more power plane
> capacitance as time goes on. The entire Power Distribution System gets
> involved if the signal current is long enough in time duration. So the
> question we should be asking is about the impedance of the PDS measured at
> the points on each power plane where the signal return path discontinuity
> occurs, and we would like to know these impedances in the important frequency
> bands. How does the PDS impedance compare to that of the 50 Ohm trace? At
> DC, kHz and MHz bands, the PDS will most likely be in the mOhms and it will
> be quite strong compared to the 50 Ohm trace. In the GHz band, the impedance
> of the PDS will be low as long as the dielectric thickness from power to
> ground plane is small. But in the stackups mentioned in this thread, some of
> the power planes are quite far from the ground plane so the plane capacitance
> and impedan
> ce suffers. Still, the PDS is likely to be much stronger than the 50 Ohm
> trace so power plane bounce will be minimal.
>
> But watch out if 100 traces cross the plane cut, particularly if they can
> switch the same direction at the same time. This potentially causes a huge
> SSN problem. 100 traces in parallel have an equivalent impedance of 50/100 =
> 0.5 Ohms and are likely to be a challenge for the PDS impedance in the GHz
> band. The voltage regulator and decoupling capacitors should be able to
> handle the return current in lower frequency bands but much crosstalk will
> occur because of power plane bounce in the GHz band.
>
> In reality, there will probably be a number of traces that is greater than 1
> but less than 100 crossing the plane cut so analysis will have to be done to
> figure out the damage. Do we care about high frequency glitches coupled from
> aggressor to victim lines? How important is rise time degradation and EMI?
> These are the important considerations in this problem.
>
> Regards,
> Larry Smith
> Qualcomm
>
> -----Original Message-----
> From: si-list-bounce@xxxxxxxxxxxxx<mailto:si-list-bounce@xxxxxxxxxxxxx>
> [mailto:si-list-bounce@xxxxxxxxxxxxx<mailto:si-list-bounce@xxxxxxxxxxxxx>] On
> Behalf Of Lee Ritchey
> Sent: Tuesday, November 08, 2011 4:59 PM
> To: Mark Grobman; Havermann, Gert
> Cc: si-list@xxxxxxxxxxxxx<mailto:si-list@xxxxxxxxxxxxx>
> Subject: [SI-LIST] Re: AW: Re: Some reference on reference planes
>
> Wow! This one has taken on a life of its own!
>
> Couple of things gleaned from building test PCBs to find out what happens
> when traces cross cuts in planes as well as hundreds of high performance
> PCBs.
>
> First, there is no good reason to cut a ground plane, so that should be the
> mechanism that ties all other things together.
>
> Second, when the PDS has been properly designed, the ripple on Vdd will be
> low enough that it is within the noise budget of signals routed over it, so
> there is no reason not to route signals over Vdd and use it as a reference
> plane.
>
> Third, the only planes that should ever be cut are Vdd planes to allow more
> than one Vdd to use the same plane. These cuts do not need to be wider than
> 10 mils to satisfy isolation and fabrication needs. When this is done and
> the two Vdds on either side of the cut are properly designed, there is an
> "AC" path across the cut created by the two Vdd supplies that render the cut
> essentially invisible to signals crossing it. I've got several test PCBs
> that validate this. Some of the measurements are in one of my books and
> others are presented in my classes. There is no need to place capacitors
> across these gaps. The PDS has already done this.
>
> Now, all of this comes unraveled if the PDS design has not been done well or
> if the ground planes have been cut. There other things that come unraveled
> as well, such as EMI and stable operation.
>
> This PDS design issue has become one of the hot topics of late as witnessed
> by all the papers presented at DesignCon. Few if any applications notes
> provide accurate advice on how to do this right. To this end, Todd Hubing,
> when he was at University of Missouri Rolla, did several tests and analyses
> and published the results as far back ad 1995. His specialty was EMI, but
> he knew that the source of much EMI was an improperly designed PDS arrived
> at by following applications notes. Yet, applications notes still don't
> incorporate these findings.
>
> Hope this helps.
>
> Lee
>
> --------------------------------------------------
> From: "Mark Grobman"<markgrobman@xxxxxxxxx<mailto:markgrobman@xxxxxxxxx>>
> Sent: Tuesday, November 08, 2011 1:21 PM
> To: "Havermann,
> Gert"<Gert.Havermann@xxxxxxxxxxx<mailto:Gert.Havermann@xxxxxxxxxxx>>
> Cc:<si-list@xxxxxxxxxxxxx<mailto:si-list@xxxxxxxxxxxxx>>
> Subject: [SI-LIST] Re: AW: Re: Some reference on reference planes
>
>> Ok, at the risk of being naive, I would like to try to put in some
>> numbers:
>> Most of my signals have a 0.5ns rise time. assuming a dielectric constant
>> of 4 that would mean signal velocity of 2Exp10 Cm/Sec (sorry for using
>> metric units). I assume that the highest relevant harmonic is at ~ 10GHz
>> so
>> my wavelength is about ~2cm.
>> Now we come to the tricky part of trying to evaluate how long is the
>> discontinuity - since the currents return to the rightful owner near the
>> BGA package and the pitch is 0.8mm than we roughly ar the vicinity of the
>> 1/4 wavelength.
>> According to this calculation the situation isn't brilliant but it's also
>> not apocalyptic - I mean the edges might smooth out a bit but on the whole
>> the signal will be ok.
>>
>> Then there is the question of crosstalk - I don't know how bad that would
>> be but the suggestion that Paul gave about adding decoupling caps between
>> the real ref planes and the ones the signal uses seems to help the
>> situation.
>>
>> I could add that we have a previous board with slightly slower freq. that
>> ha×' a similar stackup and it works fine on all accounts.
>> I would also stress that this is not a matter of economy of layers\money -
>> the small aspect ratio of via's caused by board thickness is a real
>> problem
>> and causes boards to fail.
>>
>> any more ideas? Doesn't this problem exist in other places where there
>> exist a constraint of board thickness and the necessity for many signal
>> and
>> different power layers?
>>
>> Thanks again for all the replys'
>> Mark
>>
>>
>>
>>
>> On Tue, Nov 8, 2011 at 11:21 AM, Havermann, Gert
>> <Gert.Havermann@xxxxxxxxxxx<mailto:Gert.Havermann@xxxxxxxxxxx>
>>> wrote:
>>> Hi Mark,
>>>
>>> With the chosen stack and without the ability to simulate 3D you are
>>> pretty screwed. You absolutely have to provide a clean GND return path.
>>> This is easy with ref-planes directly attached, but without it is (in 99%
>>> of the cases) too complicated to do "by hand". There are no proven rules
>>> of
>>> thumb or design practice for these odd designs.
>>>
>>> The only thing (besides adding Layers) you could do is to think yourself
>>> into the signal path to find out:
>>> - what are the reference planes for the signal?
>>> - what differential and single ended impedance will the wave see based on
>>> the reference planes?
>>> - where is the shortest possible GND path along the electric field of the
>>> signal?
>>> - what is the electrical and length difference between signal and GND
>>> path?
>>>
>>> With a lot of thinking and calculation, you might be able to get an
>>> answer
>>> to your problem, but if there are many signals involved I doubt you can
>>> make it (Murphy will play against you).
>>>
>>> Regarding you questions:
>>> The risetime isn't setting the limit, it's the GND-return discontinuity.
>>> The shorter the discontinuity, the lower the risetime can be. If the
>>> electrical length difference between the signal trace and GND retun path
>>> exceeds 1/4 wavelength, you will be in trouble.
>>>
>>> I the worst case, you will have to worry about interferences all across
>>> the board. E.g. if return currents are forced to cross thru ICs, you will
>>> face strange behavior of a component while it's the PCB that's making the
>>> error. You also open the door for all kind of EMC problems that you might
>>> not find in the Lab, but they will hit you in the field.
>>>
>>> Good Luck
>>> Gert
>>>
>>>
>>>
>>> --------------------------------------------------------------------------
>>> Absender ist HARTING Electronics GmbH& Co. KG; Sitz der Gesellschaft:
>>> Espelkamp; Registergericht: Bad Oeynhausen; Register-Nr.: HRA 5596;
>>> persönlich haftende Gesellschafterin: HARTING Electronics Management
>>> GmbH;
>>> Sitz der Komplementär-GmbH: Espelkamp; Registergericht der
>>> Komplementär-GmbH: Bad Oeynhausen; Register-Nr. der Komplementär-GmbH:
>>> HRB
>>> 8808; Geschäftsführer: Edgar-Peter Duening, Torsten Ratzmann, Dr.
>>> Alexander
>>> Rost
>>> -----Ursprüngliche Nachricht-----
>>>
>>> Von: si-list-bounce@xxxxxxxxxxxxx<mailto:si-list-bounce@xxxxxxxxxxxxx>
>>> [mailto:si-list-bounce@xxxxxxxxxxxxx<mailto:si-list-bounce@xxxxxxxxxxxxx>]
>>> Im Auftrag von Mark Grobman
>>> Gesendet: Dienstag, 8. November 2011 05:46
>>> An: Jory McKinley
>>> Cc: Rick Collins; si-list@xxxxxxxxxxxxx<mailto:si-list@xxxxxxxxxxxxx>
>>> Betreff: [SI-LIST] Re: Some reference on reference planes
>>>
>>> Hey all,
>>> I'm sorry - it seems I've confused all you (perhaps this is a reflaction
>>> of my own confusion).
>>> my stackup is 18 layers and is perfectly symmetrical. The stackup I wrote
>>> down is a "zoom" on the problematic area just so you could understand
>>> where
>>> my problem is.
>>>
>>> As for the combining of power planes: As I stated - the situation cannot
>>> be avoided without increasing the number of layers ( i tried combining
>>> but
>>> it doesn't work) which I am reluctant to do due to reliablity issues
>>> caused
>>> by the via's aspect ratio.
>>>
>>> What I really want to understand is: If I was making a DC board than we
>>> wouldn't be having this discussion. Since this is a digital board life
>>> isn't so simple (don't tell any DC engineers I implied their job was
>>> easy)
>>> - what is the area of rise times where problems start surfacing?
>>> Can I help mitage this issue *without *changing the stackup?
>>> And should I worry about interfernces throughout the transmission line or
>>> just near the edges/where the via's are?
>>>
>>> Thanks again for all the help,
>>> Mark
>>>
>>>
>>> On Tue, Nov 8, 2011 at 3:17 AM, Jory
>>> McKinley<jory_mckinley@xxxxxxxxx<mailto:jory_mckinley@xxxxxxxxx>
>>>> wrote:
>>>> Hello Mark,
>>>> Assuming you have meaningful energy on this trace, I would highly
>>>> recommend modifying your stack which seems to be unbalanced without
>>>> appropriate ground planes. The single ground plane at the bottom of
>>>> your stack is not recommended and could create all sorts of unwanted
>>>> resonances as your return current jumps to the bottom through power
>>>> cavities. I would look to pair your power planes and combine on two
>>>> of the layers not four as you have. I would either add another layer
>>>> and sandwich 3 grounds OR remove a layer and have the other layer
>>>> another ground. I do not like power on top or bottom due to potential
>>> radiation. Something like:
>>>> TOP/LowSpeed Signal 3
>>>> Power 1(Real Ref.)/Power2
>>>> GND
>>>> Signal 1
>>>> Signal 2
>>>> GND
>>>> Power 3/Power4
>>>> BOTTOM/LowSpeed Signal 3
>>>>
>>>> The potential issues you face with improper return path can create
>>>> signal integrity and timing issues on your path and potential
>>>> resonances through the power cavities. You will not only have to
>>>> decouple near the TX and RX of the path from reference to ground but
>>>> also decouple very close to the via transitions of your trace.
>>>>
>>>> -Jory
>>>>
>>>>
>>>>
>>>> ------------------------------
>>>> *From:* Mark Grobman<markgrobman@xxxxxxxxx<mailto:markgrobman@xxxxxxxxx>>
>>>> *To:* Rick Collins<gnuarm.2006@xxxxxxxxx<mailto:gnuarm.2006@xxxxxxxxx>>
>>>> *Cc:* si-list@xxxxxxxxxxxxx<mailto:si-list@xxxxxxxxxxxxx>
>>>> *Sent:* Monday, November 7, 2011 4:40 PM
>>>>
>>>> *Subject:* [SI-LIST] Re: Some reference on reference planes
>>>>
>>>> Thanks for the quick reply's.
>>>> Paul - I read in Bogatain's book that this method is not effective -It
>>>> was mentioned under what happens when you run over a gap in the return
>>>> plane but as I understand the physics is essentilay the same. To the
>>>> best of my understanding the current will "find it's way back" in a
>>>> radiative manner so that as long as the capacitance between the
>>>> relevent planes is suffiecnt it should be ok above a certain rise
>>>> time -
>>> I just don't know the numbers.
>>>> Is this method effective from your experince? what's the range of Rt
>>>> for which it works.
>>>>
>>>> Rick - Your absoulty right. I've been a bit vauge. The setup I'm
>>>> talking
>>>>> about is something like this:
>>>>>
>>>> Power 1(Real Ref.)
>>>> Signal 1
>>>> Power 2
>>>> Signal 2
>>>> Power 3
>>>> Signal 3
>>>> Power 4(GND)
>>>>
>>>> And the relevent Signal layer is "Signal 2". The distance between
>>>> different layers is 5 mil on each side.
>>>>
>>>> Mark
>>>>
>>>> On Mon, Nov 7, 2011 at 11:24 PM, Rick
>>>> Collins<gnuarm.2006@xxxxxxxxx<mailto:gnuarm.2006@xxxxxxxxx>>
>>>> wrote:
>>>>
>>>>> I recall from a course I took that if the plane of the stripline is
>>>>> tightly coupled to the reference plane, you should not have a
>>>>> problem. But "tightly coupled" may not be what you have. I think
>>>>> the context of what I learned was when there was a separation in a
>>>>> power plane or even a signal passing across a gap between two
>>>>> separate power planes, but in both cases the power planes were
>>>>> opposite a ground plane and so were "tightly coupled" acting just
>>>>> like the ground plane.
>>>>>
>>>>> Where is your driver's "reference plane" that it does not interact
>>>>> with the signal? Can you give us a better picture of what you are
>>>>> designing rather than talking in the abstract?
>>>>>
>>>>>
>>>>> At 04:15 PM 11/7/2011, Mark Grobman wrote:
>>>>>> Hello experts,
>>>>>> I require some help on the subject of reference planes. I'm
>>>>>> designing a board and despite my best efforts i'm stuck with a
>>>>>> situation where I'm forced to conduct a signal using a stripline
>>>>>> neither of whose planes are the reference planes of the signal's
>>>>>> driver (not the driver's ground or VCC).
>>>>>>
>>>>>> Now I know from various App. notes and books that this sort of
>>>>>> situation should be avoided and that I have been a bad engineer
>>> indeed.
>>>>>> Still, assuming the situation cannot be avoided I was hoping to
>>>>>> get some quantitative approximation to how bad of an idea this
>>>>>> is.Sadly speaking I don't have access to a 3d simulator which can
>>>>>> give me exact results so I'm going for best effort design methods.
>>>>>> I would love to get your input on the following issues:
>>>>>>
>>>>>> 1. Does the interference caused by not using the correct ref.
>>>>>> planes
>>>> carry
>>>>>> throughout the transmission line or does it occur only at the edges
>>>> where
>>>>>> the current "jumps" back to the correct ref. planes?
>>>>>> 2. Is there a merit figure of RiseTime/planes capacitance/???? for
>>>> which
>>>>>> the situation isn't problematic?
>>>>>> 3. Will using diff. lines improve the situation?
>>>>>> 4. Suggested reading on the matter.
>>>>>> 5. Highly insightful remarks which will blow my mind.
>>>>>>
>>>>>> Cheers,
>>>>>> Mark
>>>>>>
>>>>>>
>>>>>> ------------------------------------------------------------------
>>>>>> To unsubscribe from si-list:
>>>>>> si-list-request@xxxxxxxxxxxxx<mailto: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<mailto:si-list-request@xxxxxxxxxxxxx>
>>>>>> with 'help' in the Subject field
>>>>>>
>>>>>>
>>>>>> List technical documents are available at:
>>>>>> http://www.si-list.net
>>>>>>
>>>>>> 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<mailto: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<mailto:si-list-request@xxxxxxxxxxxxx> with
>>>>> 'help' in the Subject field
>>>>>
>>>>>
>>>>> List technical documents are available at:
>>>>> http://www.si-list.net
>>>>>
>>>>> 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<mailto: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<mailto:si-list-request@xxxxxxxxxxxxx> with
>>>> 'help' in the Subject field
>>>>
>>>>
>>>> List technical documents are available at:
>>>> http://www.si-list.net
>>>>
>>>> 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<mailto: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<mailto:si-list-request@xxxxxxxxxxxxx> with
>>> 'help' in the Subject field
>>>
>>>
>>> List technical documents are available at:
>>> http://www.si-list.net
>>>
>>> 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<mailto: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<mailto:si-list-request@xxxxxxxxxxxxx> with
>>> 'help' in the Subject field
>>>
>>>
>>> List technical documents are available at:
>>> http://www.si-list.net
>>>
>>> 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<mailto: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<mailto:si-list-request@xxxxxxxxxxxxx> with
>> 'help' in the Subject field
>>
>>
>> List technical documents are available at:
>> http://www.si-list.net
>>
>> 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<mailto: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<mailto:si-list-request@xxxxxxxxxxxxx> with
> 'help' in the Subject field
>
>
> List technical documents are available at:
> http://www.si-list.net
>
> 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<mailto: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<mailto:si-list-request@xxxxxxxxxxxxx> with
> 'help' in the Subject field
>
>
> List technical documents are available at:
> http://www.si-list.net
>
> 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 technical documents are available at:
> http://www.si-list.net
>
> 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
>
>
>
--
Steve Weir
IPBLOX, LLC
150 N. Center St. #211
Reno, NV 89501
www.ipblox.com
(775) 299-4236 Business
(866) 675-4630 Toll-free
(707) 780-1951 Fax
------------------------------------------------------------------
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.net
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
Other related posts:
