[SI-LIST] Re: Questions on Reference Planes for DDR3 signals
- From: steve weir <weirsi@xxxxxxxxxx>
- To: si-list@xxxxxxxxxxxxx
- Date: Thu, 05 Jul 2012 18:42:34 -0700
On 7/5/2012 4:23 PM, Vinu Arumugham wrote:
> Steve,
>
> Let's leave out the component/PCB interface for now and consider a
> simple 3-conductor flat ribbon cable for the transmission line
> connecting the TX to the terminations. The center conductor is the
> signal, Vdd and Vss one on each side of the signal. Signal/Vss and
> Signal/Vdd each having a characteristic impedance of 100 ohm.
>
> Do you agree that the above transmission line when used in the SRS
> configuration I described will result only in DC draw from the supply?
No, I do not.
>
> I am not sure what you mean by continuous transmission line signaling
> system but the properties you describe seem to apply to what I described
> as SRS.
This has been expressed different ways over the past 25 years. There
was a Design Con 2012 paper that dealt with this old idea that some
think is new again.
> If we define SSN as noise caused when multiple buffers/terminations
> share a common PDN impedance, SRS will avoid this noise.
Again, I disagree for the reasons I have stated: When the AC signal
current transitioning an interface is non-zero, then the return current
through the common impedance of that interface is also non-zero, and by
definition the result is SSN.
>
> If we now compare the practical implementation of conventional signaling
> and SRS, the question becomes how much of the margin we gained from the
> lack of SSN do we have to give up. The answer will determine if SRS is
> useful in practice.
Again, if we look at the five rings of EMC hell, we find that using
multiple transmission lines in parallel, each coupling to planes on
independent DC rails and therefore coupled through capacitors will never
be better than using single transmission lines that reference a single
rail, and will usually be much worse.
> In conventional signaling we try to keep a constant signal/Vss impedance
> end-to-end. In SRS we have do that for Signal/Vss and Signal/Vdd.
Yes, but as I have attempted to explain, all that does for you in the
best case is divide the common impedance that the SSN forms across in
half. In practice, depending on the distribution of impedance in each
rail, it can make it much worse than alternatives.
> Thanks,
> Vinu
>
>
> On 07/02/2012 06:28 PM, steve weir wrote:
>> Vinu, the problem is this: At the boundary of the component to the PCB,
>> the signal forms two transmission lines that each carry the same
>> polarity transitions with respect to each of the image planes. That
>> transition carries through the shared impedance of each of the
>> respective rails between the package and the PCB. Voltage developed
>> across those shared impedances is the stuff that SSO is made of.
>>
>> I think that you have confused this configuration with the notion of a
>> continuous transmission line signaling system. In a continuous
>> transmission line signaling system the DC current is constant and
>> hypothetically, the AC current approaches zero. An ideal differential
>> signaling system has that behavior. In such a system, signaling is done
>> by changing the current distribution between lines, but not the total
>> current. If the lines are all close together then the approximation to
>> the ideal can be pretty good. But that is a very different beast than
>> what I believe you have been describing.
>>
>> If we want to approach zero AC current in the power distribution
>> interconnect, then the even mode signal current must approach zero.
>>
>> Best Regards,
>>
>>
>> Steve.
>> On 7/2/2012 5:05 PM, Vinu Arumugham wrote:
>>> Steve,
>>>
>>> May be we should temporarily set aside practical considerations. If you
>>> had an SRS configuration with three wires, Vddq/signal/Vss, do you agree
>>> that it will steer current and only draw DC from the supply? In contrast
>>> any other configuration would draw pulsed current from the supply.
>>>
>>> Thanks,
>>> Vinu
>>>
>>> On 06/27/2012 06:53 PM, steve weir wrote:
>>>> Vinu, there seems to be some discussion at cross purposes going on. If
>>>> we reference a signal to two different planes then the coupled energy
>>>> has to make it end to end. At the die launch we can rely on die
>>>> capacitance to provide the necessary driver coupling. Then under a
>>>> first assumption that we approximate equal coupling between each signal
>>>> and both rails, and that we introduce only equal inductance between the
>>>> die Vddq, and Vss through the package and into the PCB, we can then turn
>>>> our attention to the PCB part of the channel. And this is where it
>>>> looks like we are having multiple conversations.
>>>>
>>>> Let's start with a simple case where there is a single stripline
>>>> cavity. The signal energy that we launch into that cavity will excite
>>>> it. The cavity once excited will resonate at modal frequencies. If we
>>>> want to drive those frequencies up, then we can beak the cavity up into
>>>> smaller effective cavities, smaller beer cans if you will by stitching.
>>>> Because the two rails require DC isolation, we cannot stitch with vias
>>>> that connect the two planes together. We will have to stitch through
>>>> capacitors, which today means returning all the way to the surface and
>>>> back with vias. If the cavity is in the middle of an .062 PCB and we
>>>> use regular MLCCs then we are talking about 1nH or more loop inductance
>>>> per capacitor. For signals with 100ps Tr, which has an Fknee near 3GHz,
>>>> those capacitors look like 20 Ohms or so. In order to look like a low
>>>> impedance compared to the cavity necessary to affecct the resonances, we
>>>> are going to need a lot of capacitors densely packed. If we don't tame
>>>> the resonances, then signals that excite them get the favor returned by
>>>> the resulting voltages coupling back into the signals, as well as
>>>> setting up EMI headaches.
>>>>
>>>> Now, if we take the same stripline and make both planes Vss, then we can
>>>> stitch together with vias. The resulting impedance will be much lower,
>>>> as well as the required real estate per short. One via effects a short
>>>> instead of a via pair throughout the PCB, in addition to the surface
>>>> area of the bypass caps. It's a completely different and far more
>>>> manageable problem.
>>>>
>>>> Best Regards,
>>>>
>>>>
>>>> Steve
>>>> On 6/27/2012 4:38 PM, Vinu Arumugham wrote:
>>>>> I was talking about reducing injection by providing return vias for both
>>>>> planes, not about suppression.
>>>>>
>>>>> Thanks,
>>>>> Vinu
>>>>>
>>>>> On 06/27/2012 01:16 PM, Scott McMorrow wrote:
>>>>>> Vinu,
>>>>>>
>>>>>> sorry, wrong answer.
>>>>>>
>>>>>> So, one vss via dangling in the cavity
>>>>>> One vdd via dangling in the cavity
>>>>>> how is the AC short necessary to suppress cavity waves made?
>>>>>>
>>>>>> you have wrong ideas regarding what a via can do when only connected
>>>>>> to one net.
>>>>>>
>>>>>> Scott
>>>>>>
>>>>> ------------------------------------------------------------------
>>>>> 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
>
>
>
--
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
All contents Copyright (c)2012 IPBLOX, LLC. All Rights Reserved.
This e-mail may contain confidential material.
If you are not the intended recipient, please destroy all records
and notify the sender.
------------------------------------------------------------------
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
Other related posts:
