[SI-LIST] Re: DDR2 2-slot design preference...
- From: Scott McMorrow <scott@xxxxxxxxxxxxx>
- To: Jory McKinley <jory_mckinley@xxxxxxxxx>
- Date: Wed, 31 Oct 2007 13:24:25 -0400
Jory
The electrical length of a via penetrating a cavity controls the amount
of energy injected into the cavity at any particular frequency. The
shorter the cavity crossing, the less energy injected, but energy is
nonetheless injected. An NRZ signal running a random pattern will have
signal energy drop off at a 20 dB/decade slope, until the Knee
frequency, where it drops off more rapidly. Up until you reach the
knee, you have to worry. As a result, there are significant signal
harmonics for even a 200 ps rise/fall time signal out to 1.75 GHz.
For example, a DDR2 500 memory system will have signal energy at 250
MHz, 750 MHz and 1.25 GHz. These are frequencies where it is quite easy
to build cavity resonances and parallel resonances in a PCB. Even the
slightest amount of energy coupled into the cavity is multiplied by the
large number of transitions that occur.
Let's say that 1 mV of noise is coupled from 1 DDR signal into a cavity
and rattles around. Now transition 128 signals simultaneously on a
double wide bus, and you've got 128 mV. What if the cavity resonates at
a particular frequency within the signal spectrum? If you excite that
frequency with a repetitive pattern, it is possible to pump up the
cavity, in which case you will easily see 2X, 4X or more of the original
injected noise, since planar cavities are not very lossy below a few GHz.
If there are return path vias in the proximity of the signal vias, then
there is considerable energy containment. For ground-power transitions
that means that there needs to be ample bypass devices of sufficiently
low inductance to capture the energy, and the cavity height needs to be
sufficiently small to reduce the amount of energy coupled.
Unfortunately, it is sometimes the case that between memory controllers
and memory devices that additional signal transitions occur without
nearby bypass stitch vias or ground stitch vias. In that case,
significant energy can be coupled into these inadvertent resonant
circuits, resulting in increased power noise and signal crosstalk. This
is not generally a huge issue for differential signals, since there is
significant common mode cancellation, but can be a big problem for large
single-ended buses.
regards,
Scott
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
Jory McKinley wrote:
> Taking a step back on this one...........How we look at a via
> structure depends on the electrical length of the via structure versus
> the edge rate of the signals traveling through the via structure.
> Most via's we are dealing with have an electrical length in the 10ps -
> 30ps range. The question is at what point can this via structure
> create potential EMI/SI/resonance issues? It depends on the edge rate
> of the signals traveling through the via structure. For example edge
> rates above 200ps hitting a typical via structure will encounter LRC
> effect given a reasonable via ground return (If no via ground return
> we may excite some cavity resonance). In reading most of this thread
> it would appear that we are talking about edge rates in the 50ps -
> 150ps range where full wave physics comes into play in a typical via
> structure.
> -Jory
>
> ----- Original Message ----
> From: Scott McMorrow <scott@xxxxxxxxxxxxx>
> To: vinu@xxxxxxxxx
> Cc: eric@xxxxxxxxxxxxxxx; pritchard_jason@xxxxxxx; si-list@xxxxxxxxxxxxx
> Sent: Tuesday, October 30, 2007 9:52:02 PM
> Subject: [SI-LIST] Re: DDR2 2-slot design preference...
>
> Vinu
> Unfortunately you cannot apply a transmission line approximation to
> signal and ground via sets. When a signal "turns the corner" and heads
> down a signal via, a very complex set of interactions occur against all
> of the local boundaries.
>
> 1) part of the wave detaches from the trace and surrounds the via.
>
> 2) simultaneously part of the wave detaches from the plane(s) it is
> referenced to and heads down the rabbit hole through the via antipad
> opening.
>
> 2a) For stripline, there is one signal via and two openings in the
> plane, in which case the signal path splits and waves squirt up and down
> through the holes. When this happens the return path is majorly messed
> up causing a conversion to the parallel plate mode of the cavity, with a
> circular wave front developing that propagates outward in all directions
> from the via in the center.
>
> 3) If there are ground vias across the cavity in the vicinity of the
> signal via, then part of the cavity is shorted, and some of the parallel
> plate mode energy is returned back down towards the plane in the
> direction of the signal travel.
>
> 4) One can simplify modeling of the behavior of a signal traveling on a
> via as it passes through two planes in this manner, with a ground via
> nearby, as the inductance and capacitance of this new transmission line
> segment, but that is an oversimplification.
>
> 5) If you are transitioning single-ended signals through vias, and you
> forget to stitch the planar cavities, you end up with all that
> parallel-plate energy rattling around. Just like our friend, the
> Wack-a-Mole(tm) it can and will pop up all over the place.
>
> Eric is quite correct in his description. And he's quite correct about
> his assumption about coaxial ground vias surrounding a signal via. Take
> a look at a good SMA launch pattern, or a good microstrip to via launch
> pattern. There is more than impedance tuning going on.
>
> Regards,
>
> Scott
>
>
> 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
>
>
>
> Vinu Arumugham wrote:
> > Eric,
> >
> > Unless I misunderstood, your description of the return via below
> does not seem to be accurate.
> > The signal via and return via(s) form a transmission line. One can
> of course tune the impedance of the signal via by changing the spacing
> and number of return vias. I don't think it is accurate to use the
> lumped inductance value and say that the return via has a series
> impedance of 6 ohm at 1GHz.
> > The noise injected into the planes by the return via(s) should be
> mostly canceled due to the noise injected by the signal via.
> >
> > "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."
> >
> > Thanks,
> > Vinu
> >
> >
> > Eric Bogatin wrote:
> >
> >> 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 <mailto:eric@xxxxxxxxxxxxxxx>
> >> www.BeTheSignal.com <http://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>
> [mailto:si-list-bounce@xxxxxxxxxxxxx
> <mailto:si-list-bounce@xxxxxxxxxxxxx>] On
> >> Behalf Of pritchard_jason@xxxxxxx <mailto:pritchard_jason@xxxxxxx>
> >> Sent: Tuesday, October 30, 2007 1:58 PM
> >> To: Chris.Cheng@xxxxxxxx <mailto:Chris.Cheng@xxxxxxxx>;
> si-list@xxxxxxxxxxxxx <mailto: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
> <mailto:Chris.Cheng@xxxxxxxx>]=20
> >> Sent: Tuesday, October 30, 2007 2:40 PM
> >> To: pritchard, jason; si-list@xxxxxxxxxxxxx
> <mailto: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>
> >> [mailto:si-list-bounce@xxxxxxxxxxxxx
> <mailto:si-list-bounce@xxxxxxxxxxxxx>]On Behalf Of
> >> pritchard_jason@xxxxxxx <mailto:pritchard_jason@xxxxxxx>
> >> Sent: Tuesday, October 30, 2007 10:32 AM
> >> To: si-list@xxxxxxxxxxxxx <mailto: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
> <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
> >> 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
> <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
> >> 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 <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
> > 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 <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
> 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
>
>
>
>
> __________________________________________________
> Do You Yahoo!?
> Tired of spam? Yahoo! Mail has the best spam protection around
> http://mail.yahoo.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 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:
