[SI-LIST] Re: DDR2 2-slot design preference...
- From: Scott McMorrow <scott@xxxxxxxxxxxxx>
- To: leeritchey@xxxxxxxxxxxxx
- Date: Tue, 30 Oct 2007 23:43:16 -0400
Yep, aren't differential pairs nice? They minimize the amount of energy
injected into the cavity. Try 1 or 2 Gbps single-ended data transfers
and then you'll start seeing cavities light up. As I said previously,
it's a matter of the magnitude of the signals that are coupled into the
cavity.
Scott McMorrow
Teraspeed Consulting Group LLC
121 North River Drive
Narragansett, RI 02882
(401) 284-1827 Business
(401) 284-1840 Fax
http://www.teraspeed.com
Teraspeed® is the registered service mark of
Teraspeed Consulting Group LLC
Lee Ritchey wrote:
> We are still talking about simulations. The real question isn't is there
> some coupling mechanism, but rather is the coupled energy significant.
> It's just like the via in a signal path question. It is certainly visible,
> but it does not contribute significant signal degradation.
>
> For example we just finished a supercomputer that has thousands of 5.2 Gb/S
> paths in it all of which have 4 vias in each path. There is a visible
> reflection from each via, but these reflections are so small their impact
> on signal quality is tiny compared to skin effect loss and dielectric loss.
>
>
>
>> [Original Message]
>> From: Eric Bogatin <eric@xxxxxxxxxxxxxxx>
>> To: <pritchard_jason@xxxxxxx>; <si-list@xxxxxxxxxxxxx>
>> Date: 10/30/2007 3:41:40 PM
>> Subject: [SI-LIST] Re: DDR2 2-slot design preference...
>>
>> Guys-
>>
>> I'll add two observations to this discussion on planes, vias and
>>
> resonances.
>
>> I've been doing a lot of via design and simulation work with a 3D planar
>> tool. I've had to re-adjust my intuition about the role of adjacent return
>> vias and noise injection into cavities.
>>
>> As previously noted, the efficiency of injecting noise into the plane to
>> plane cavity is related to the impedance of the cavity, which, to first
>> order is about the spacing between the planes. The thinner the dielectric,
>> the lower the impedance, and the less coupled energy driving the plane
>> resonances.
>>
>> You get far more reduction in coupling to the cavity mode by thinner
>> dielectric than by adding the return via. If the spacing between the
>>
> planes
>
>> is thin, there is less vertical distance to couple between and the plane
>> impedance is lower.
>>
>> In a large board, there will always be adjacent planes in the return path
>> with a large spacing and this is the pair where cavity resonances will be
>> excited.
>>
>> Secondly, having an adjacent return via does not suppress the coupling
>>
> into
>
>> the cavity. It reduces it by maybe 50%, depending on the spacing to the
>> signal via and its length. It is not enough to eliminate the noise
>>
> coupling
>
>> into the plane to just have a return via adjacent to the signal via. You
>>
> may
>
>> need a few. How many do you need? Of course, the answer is "it depends."
>>
>> The rule of thumb is best articulated by my good friend Frank Schonig who
>> says, "A lot is good, more is better and too much is just right." I
>>
> haven't
>
>> done the analysis, but I suspect that the more coaxial the return via
>> arrangement looks to the signal via, the less total inductance in the
>>
> return
>
>> path and the less the radiated coupling into the plane to plane cavity
>> resonance.
>>
>> Of course it is not practical to add 4 return vias around each signal via,
>> unless you are doing a very low density, high isolation board, like a test
>> board or a load board. Everything else is going to be a compromise.
>>
>> If you are not going to do a detailed 3D planar simulation of the return
>> plane stack up and the return via configuration to simulate how much
>> insertion loss you loose into the planes, you will want to add design
>> margin, like by adding vias along the edge, and multiple return vias in
>> close proximity to the signal vias.
>>
>> Keep in mind that a return via is not an ideal short. It has a finite
>> impedance. As a rough rule of thumb, its total inductance per length is
>> about 10 pH/mil. If the return via is 100 mils long, it has 1 nH of total
>> inductance. At 1 GHz, this is an impedance of 6 Ohms. If you have 1 return
>> via per signal via, the ground bounce across it, which would be a voltage
>> source, injecting noise into the planes, would be about 10% of the signal
>> swing voltage.
>>
>> --eric
>>
>>
>> **************************************
>> Dr. Eric Bogatin, President
>> Bogatin Enterprises, LLC
>> Setting the Standard for Signal Integrity Training
>> 26235 w 110th terr
>> Olathe, KS 66061
>> v: 913-393-1305
>> f: 913-393-0929
>> c:913-424-4333
>> e:eric@xxxxxxxxxxxxxxx
>> www.BeTheSignal.com
>> Spring 2008 Signal Integrity Training Institute
>> EPSI, SIAA, BBDP
>> April 7-11, 2008, San Jose, CA
>> ****************************************
>>
>> -----Original Message-----
>> From: si-list-bounce@xxxxxxxxxxxxx [mailto:si-list-bounce@xxxxxxxxxxxxx]
>>
> On
>
>> Behalf Of pritchard_jason@xxxxxxx
>> Sent: Tuesday, October 30, 2007 1:58 PM
>> To: Chris.Cheng@xxxxxxxx; si-list@xxxxxxxxxxxxx
>> Subject: [SI-LIST] Re: DDR2 2-slot design preference...
>>
>> Yes 1 ground via was placed directly next to each the signal vias on the
>> test board. They were 100 ohm vias. Unfortunately it kept the impedance
>> low at the edges of the via structure where the grounds were placed. You
>> would need more ground vias to truly pin it down. We did one simulation
>> with them taken out to show how it got worse.=20
>>
>> I would imagine voltage planes are more often the culprit for
>> resonances. They may be only used to supply power at one location on the
>> board and then are routed to the rest of the design as a signal
>> reference. These planes typically don't have capacitors placed across
>> the whole design. If you did have capacitors across the whole design you
>> may only have a limited frequency range in which that may be effective.=20
>>
>> -Jason
>>
>>
>>
>> -----Original Message-----
>> From: Chris Cheng [mailto:Chris.Cheng@xxxxxxxx]=20
>> Sent: Tuesday, October 30, 2007 2:40 PM
>> To: pritchard, jason; si-list@xxxxxxxxxxxxx
>> Subject: RE: [SI-LIST] Re: DDR2 2-slot design preference...
>>
>> Before I started I have to say I am also a big fan of ground via
>> stitching around edges of PCB.
>> That said. In your experiment, did you provide ground return current
>> vias near your differential pair transition via ? One can easily design
>> an experiment where return current path is denied (no ground vias near
>> the signal vias) and it is forced to return through plane coupling (i.e..
>> to justify thin core capacitance planes) or your via stitching (to
>> contain the large EMI radiation field). Neither is the correct solution
>> to the problem which is lack of return current vias.
>> Another thing to consider is in real live non-backplane PCB's, there are
>> tens of thousands of ground vias by IC's and passive components
>> sprinkled around the PCB, it will be hard to find a large piece of
>> via-less plane to start your resonance.
>>
>> -----Original Message-----
>> From: si-list-bounce@xxxxxxxxxxxxx
>> [mailto:si-list-bounce@xxxxxxxxxxxxx]On Behalf Of
>> pritchard_jason@xxxxxxx
>> Sent: Tuesday, October 30, 2007 10:32 AM
>> To: si-list@xxxxxxxxxxxxx
>> Subject: [SI-LIST] Re: DDR2 2-slot design preference...
>>
>>
>> I contributed to the paper, so I'll try and shed some light on what was
>> in it...
>>
>> The purpose of the paper was to explain how high frequency energy can
>> travel across a PCB and radiate from PCB edges or end up in areas you
>> didn't expect it to be.=3D20
>>
>> If you spend a little time in the lab taking EMI measurements then you
>> will find out that if you take any board with high speed serial links
>> with via transitions or stripline routing, and measure around the edge
>> of the PCB you will almost always find energy there. The question I
>> always had was, how did it get there? I have been doing SI for many
>> years so I typically thought about problems in 2 dimensions. The problem
>> with EMI is it's 3 dimensional. It is sometimes difficult to predict how
>> energy will travel. The first step is knowing the mechanisms in which
>> energy gets diverted and spread out across the PCB.=3D20
>>
>> The first thing we did was set-up simple experiments in SI-Wave to try
>> and figure out what was going on. We created simplified etch layouts of
>> the real board that was having problems. We soon came to the conclusion
>> that via transitions were exciting resonances on the PCB. What we
>> determined was that the size of your reference plane and the resultant
>> cavity resonances created between 2 planes caused energy to travel in
>> the direction of the resonances when excited by via transitions. This
>> loss of energy to the planes can also be seen in the s-parameters of the
>> etch. That is essentially the first half of the paper.=3D20
>>
>> We then went into the lab. The experiments were done on a backplane test
>> board. It only had ground planes. We chose this board because it had SMA
>> connections and allowed us the flexibility to apply whatever input we
>> wanted. It also had the same etch/via structures of our problem board,
>> and proves the point that it doesn't matter if its power or ground. All
>> you need is 2 metal pieces to create a cavity resonator.=3D20
>>
>> The simulations and lab measurements proved that you could predict where
>> emissions would occur on a PCB. Did this experiment actually solve a
>> real problem? Indirectly. Once we knew what mechanisms allowed energy to
>> go to unwanted places on a PCB you can change the layout to accommodate
>> this. One solution is to use via stitching along the edge of the PCB to
>> reduce the impedance so that it cant radiate. This was implemented
>> because the board slipped into metal clips at the edges of the PCB. If
>> you can squelch the noise before it gets to the metal clips you can
>> reduce the amount of energy directly coupled to the chassis. Another
>> solution would be to make sure your return path impedance is very low
>> along all of your high speed signals which is very difficult in high
>> density boards.=3D20
>>
>> You could consider via fencing along the edge of a PCB a "rule of
>> thumb", but it's a useful one because I have yet to see anyone capable
>> of looking at a PCB and tell me how the energy is going to travel across
>> the PCB, couple, and radiate. This is not a 2D SI problem its 3D.
>> Obviously you could put the work in and simulate it, but that is often
>> time consuming and not available to most people.=3D20
>>
>> We were going to present the REAL board results at design con in
>> February but it wasn't in the cards this year.=3D20
>>
>> I am not an EMI "guru". I just wanted to understand what is happening.
>> Just because you haven't seen it doesn't mean it doesn't exist.=3D20
>>
>> References:=3D20
>> * Reducing Simultaneous switching noise and emi on ground/power planes
>> by dissipative edge termination. Istvan
>> * EMI mitigation with multilayer Power Bus Stacks and via stitching of
>> reference planes. Xiaoning ye, David M. Hockanson, Min Li,.....
>> * Radiated Emission from a multilayer PCB with traces placed between
>> power/ground planes. Takashi Harada, Hideki Sasaki, Toshihide Kuriyama
>> * Reduction in radiated emission by symmetrical power-ground layer
>> stack-up pcb no open edge. Satoru Haga, Ken Nakano, Osamu Hashimoto
>> * The Radiation of a rectangular power bus structure at multiple cavity
>> mode resonances. Marco Leone
>> * Coupling of through hole signal via to power/ground references and
>> excitation of edge radiation in multilayer PCB. Jun So Pak, Jingook Kim
>> .....
>>
>> -Jason
>>
>>
>>
>>
>> This email and any attachments thereto may contain private,
>> confidential, and privileged material for the sole use of the intended
>> recipient. Any review, copying, or distribution of this email (or any
>> attachments) by others is strictly prohibited. If you are not the
>> intended recipient, please contact the sender immediately and
>> permanently delete the original and any copies of this email and any
>> attachments thereto.
>>
>> ------------------------------------------------------------------
>> 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
>> 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.net
>>
>> 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.net
>
> 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.net
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:
