They are proportioning constants. The results that one gets with method 2 versus certain variations of method 3 depend highly on geometry of the cavities and the stitch via pattern. Best Regards, Steve. On 6/27/2012 9:15 AM, Ravinder.Ajmani@xxxxxxxx wrote: > > Hi Steve, > > This may look like a dumb question, but please tell me what do X and Y > represent in your note. > > Speaking of the 5 rings of Signal Integrity/EMC hell, the only way to > accomplish #1 is to route all the signals on Top layer, which is > practically impossible. I generally use #2 in my designs, and it keeps > EMI under control. I also did some modeling to determine the effect of > ground vias, and didn't see any noticeable improvement when using #2 > routing strategy. > > Thanks. > > > Regards > Ravinder Ajmani > HGST, a Western Digital company > ravinder.ajmani@xxxxxxxx > > > > > > > > *steve weir <weirsi@xxxxxxxxxx>* > Sent by: si-list-bounce@xxxxxxxxxxxxx > > 06/27/2012 12:44 AM > Please respond to > weirsi@xxxxxxxxxx > > > > To > si-list@xxxxxxxxxxxxx > cc > > Subject > [SI-LIST] Re: Questions on Reference Planes for DDR3 signals > > > > > > > > > > Liuluping, SSO noise is almost exclusively the result of di/dt through > common inductance. Minimizing SSO requires that we minimize the product > of series inductance and di/dt from the die launch through the entire > channel. If you have X*N Vddq balls and Y*N Vss balls, the ideal > distribution is X SSO signals referenced to Vddq for every Y SSO signals > referenced to Vss. Only if X = Y will you get the lowest noise by evenly > splitting SSO di/dt between PCB Vss and PCB Vddq. In that case you have > the option of referencing half of the signals to X and half to Y or > alternately referencing all signals evenly to X and to Y. That gets you > us out of the package. > > Once we are in the PCB, every time that a signal traverses a cavity, ANY > cavity it excites that cavity. If the cavity has the same DC rail on > both planes, then we can button down the cavity with stitch vias. > Otherwise, we have to use bypass capacitors. Barring embedded > capacitors, the deeper the cavity is in the board, the harder it will be > for bypass capacitors to be effective due to the large loop inductance > imposed by the long distance between the cavity and the capacitor > mounting surface. > > So the best strategy is to: a) Avoid exciting ANY cavity, and b) Where > we excite a cavity minimize what is required to hold the disturbance to > an acceptable level. a) and b) will take us to the five types of route > classes, or as I like to say the five rings of EMC/signal integrity hell > as outlined by authors like Bruce Archambeault: > > a) Route against one surface of one plane end to end. > b) Route against the surfaces of one plane end to end. > c) Route against multiple planes that are stitched together with vias. > d) Route against multiple planes that are stitched together with bypass > capacitors, IE the two voltages of a given rail. > e) Route against multiple planes that are stitched together with series > bypass capacitors, IE unrelated voltages. > > The problem with strategy #2 is that it begins life at the fourth ring > of EMC / signal integrity hell. Whereas #1 never gets deeper than the > third rail. Within the PCB, strategy #2 will never be able to outperform > strategy #1. Noted EMC and signal integrity specialist and former First > Lady Nancy Reagan advises: "Just say no to mixed PCB return references." > > Steve. > > On 6/26/2012 8:45 PM, Liuluping wrote: > > Hi steve and all: > > Thank you for your reply; Can we consider that the strategies 2) > just separate the SSO noise in two rails instead of just one rail, > > so reduce noise on each rail, but the sum of the noise on the two > rail will equal to strategies 1)£¿ > > To make things more clear, lets consider a practical design > case(here I collect some discussion on the SI-List before, thanks to > all the people): > > A Controller with 10pcs DDR3@2133Mbps(NOT DIMM), with 160bit DQ ,20 > diff dqs, 80bit address ,20 diff clk and other signals. > > To simplify analysis,here we assume that the pin map have designed > that ,as steve suggest, have equal Lvdd and Lvss (at package). > > The board is 14 layer boards, may have two solutions: > > ************************************* > > Solution A: > > The stackup is : > > TOP > > GND02 > > ART03 > > GND04 > > ART05 > > GND06 > > PWR07 > > ART08 > > GND09 > > ART10 > > GND11 > > ART12 > > GND13 > > BOTTOM > > > > Key notes: > > 1)All DDR3 signal route in ART03/05/10/12, couple to two GND plane. > > 2)VDDIO @PWR07, the distance between GND06 and PWR07 is about 3mil. > > 3)VTT decouple to only GND. > > 4)CLK VTT is the same with 3£©. > > 5) Vref decouple to both VDDIO and GND . > > > > Advantage: all signal couple to a "clean" GND, VDDIO close couple to > GND, may be improve the SSO noise decoupling; > > Disadvantage: Double the SSO noise compare to solution B? > > > > ************************************* > > Solution B: > > The stackup is : > > TOP > > GND02 > > ART03 > > VDDIO > > ART05 > > GND06 > > PWR07 > > ART08 > > GND09 > > ART10 > > VDDIO > > ART12 > > GND13 > > BOTTOM > > > > Key notes: > > 1)All DDR3 signal route in ART03/05/10/12, couple to BOTH VDDIO and > GND plane. > > 2)VDDIO NOT at PWR07. > > 3)VTT decouple to both VDDIO and GND. > > 4)CLK with 36ohm floating terminal ,as the DIMM spec, and decouple > to VDDIO only. > > 5) Vref decouple to both VDDIO and GND . > > > > Advantage: all signal couple to both VDDIO and GND ,may half the SSO > noise at VDDIO plane?; > > Disadvantage: 1) Noisy VDDIO will reduce the margin of the signal; > > 2) VDDIO not close couple to GND, may worse the VDDIO noise? > > *************************************** > > I will choose solution A, How about your opinions? > > > > Thanks advance, > > > > LIU Luping > > > > -----ÓʼþÔ¼þ----- > > ·¢¼þÈË: steve weir [mailto:weirsi@xxxxxxxxxx] > > ·¢ËÍʱ¼ä: 2012Äê6ÔÂ26ÈÕ 20:10 > > ÊÕ¼þÈË: Liuluping > > ³ËÍ: si-list@xxxxxxxxxxxxx > > Ö÷Ìâ: Re: ´ð¸´: Questions on Reference Planes for DDR3 signals > > > > There seems to be some confusion going around about the channel on the > > PCB, and the package launch. > > > > 2) can only reduce the SSO in half under a special set of conditions. > > That's the best it can do. > > > > You can view 2) as taking N 50 Ohm lines and converting them to 2N > > paired 100 Ohm lines, one line for each that references Vss and another > > that references Vdd. If Lvdd and Lvss between the PCB and die are equal, > > then the di/dt through Lvdd and Lvss are each half what it would have > > been with N 50 Ohm lines referencing only Vdd or Vss with the same Lvss > > or Lvdd. The assumption of equal Lvss and Lvdd is questionable. It > > relies on a package designer either naively choosing the number of balls > > for each rail, or planning for this balanced stripline PCB routing. > > > > A smart package designer planning for the method 1) would allocate > > enough Vdd and Vss connections to realize appropriate Lvdd and Lvss for > > the number of lines that will reference each. So, if a memory controller > > had 24 A/C that the designer intends should reference PCB Vdd and 128 > > data lines that should reference PCB Vss, then the ball pattern should > > have a ratio of about 6 Vss for every Vdd. The key thing to remember is > > that SSO builds across shared impedance. If the shared impedance is very > > low relative to the di/dt, and there are not resonance problems, then > > the SSO will be small. A very conservative package would carry one > > signal return ball for each single ended signal ball. > > > > Signals should only make absolutely necessary reference changes. > > Differential or not, I recommend routing high speed data lines against a > > contiguous Vss reference. > > > > Steve > > On 6/26/2012 3:19 AM, Liuluping wrote: > >> Hi Steve: > >> Thank you for your quickly reply, your explain is very helpful to me. > >> As the strategies 2,coupled every thing to both rails ,you > mentioned that we have > >> half the total inductance and half the SSO amplitude, here is > compared to the stripline > >> couple to 2 vss plane or micostrip couple to 1 vss plane? > >> Further more, for the DDR4 Pseudo-Open-Drain Logic (PODL), all > signal should couple to vss,right? > >> > >> Thanks, > >> LIU Luping > >> > >> -----ÓʼþÔ¼þ----- > >> ·¢¼þÈË: steve weir [mailto:weirsi@xxxxxxxxxx] > >> ·¢ËÍʱ¼ä: 2012Äê6ÔÂ26ÈÕ 13:45 > >> ÊÕ¼þÈË: Liuluping > >> ³ËÍ: si-list@xxxxxxxxxxxxx > >> Ö÷Ìâ: Re: Questions on Reference Planes for DDR3 signals > >> > >> There are a couple of different strategies: > >> > >> 1) Couple about half the lines to Vss and the remainder to Vdd. On the > >> PCB route each line to the rail referenced end to end. This is the idea > >> used by memories today: Data to Vss, A/C to Vdd. > >> > >> 2) Couple everything to both rails. Then route stripline in proportion > >> to the coupling in the package. This theoretically can work, but is > very > >> restrictive on PCB routing. > >> > >> Lvdd and Lvss are most important at the driving end. With ODT they also > >> matter almost as much at the Rx end. Vnoise = Lcommon*di/dt still > >> defines common signal noise. Limit Lcommon, di/dt, or both to get > >> acceptable Vnoise. > >> > >> Vtt should track the AC reference(s). If only one reference is used for > >> a given signal line as in 1) then the decoupling is simpler. > >> > >> Steve > >> > >> On 6/25/2012 8:26 PM, Liuluping wrote: > >>> Hi Steve: > >>> Two places not very understand: > >>> 1¡¢For a given di/dt * N bits > >>> transitioning from low to high, relative to BOTH planes the di/dt is > >>> positive. If the interconnect is completely symmetrical then we have > >>> half the total inductance and half the SSO amplitude. > >>> -----Is it means that the VDDIO-DQ-GND stackup can half the SSO > noise compare to GND-DQ-GND ? > >>> If so ,how to trade off ,as Jeff Loyer mentioned, as the noisy > VDDQ may "eat" the margin of DQ. > >>> 2¡¢ The signal line is going high: It is drawing positive > >>> convention current through the die PDN and back to the PCB PDN > through > >>> both Lvdd and Lvss. > >>> --- Here the Lvdd and Lvss locate at receiver side,right? And if > the signal is ADD or CMD with VTT, is it better to decouple to both > GND and VDDIO? > >>> > >>> Thanks, > >>> > >>> LIU Luping > >>> > >>> ***************************************************************** > >>> This e-mail and its attachments contain confidential information from > >>> HUAWEI, which is intended only for the person or entity whose > address is > >>> listed above. Any use of the information contained herein in any way > >>> (including, but not limited to, total or partial disclosure, > reproduction, > >>> or dissemination) by persons other than the intended recipient(s) is > >>> prohibited. If you receive this e-mail in error, please notify the > sender by > >>> phone or e-mail immediately and delete it! > >>> ***************************************************************** > >>> > >>> > >>> -----Original Message----- > >>> From: si-list-bounce@xxxxxxxxxxxxx > [mailto:si-list-bounce@xxxxxxxxxxxxx] On Behalf Of steve weir > >>> Sent: Saturday, June 23, 2012 7:05 AM > >>> To: si-list@xxxxxxxxxxxxx > >>> Subject: [SI-LIST] Re: Questions on Reference Planes for DDR3 signals > >>> > >>> Vinu, a completely balanced transmission path can theoretically > divide > >>> SSO in half. It does not cancel it. Let us suppose that we have a > >>> completely balanced transmission path using a symmetrical > stripline all > >>> the way back to the die launch. For a given di/dt * N bits > >>> transitioning from low to high, relative to BOTH planes the di/dt is > >>> positive. If the interconnect is completely symmetrical then we have > >>> half the total inductance and half the SSO amplitude. We do not > cancel > >>> the SSO. The only way to cancel SSO is to code such that the > summation > >>> of transitions multiplied by polarity equals zero. > >>> > >>> Steve. > >>> > >>> Msg: #6 in digest > >>> Date: Mon, 25 Jun 2012 10:26:30 -0700 > >>> From: steve weir <weirsi@xxxxxxxxxx> > >>> Subject: [SI-LIST] Re: Questions on Reference Planes for DDR3 signals > >>> > >>> On 6/25/2012 10:02 AM, Vinu Arumugham wrote: > >>>> Steve, > >>>> > >>>> One can view it as two t-lines - signal/Vdd and signal/Vss - both > with > >>>> the same characteristic impedance and both terminated at their > >>>> characteristic impedance - say 100 ohm. > >>> Yes, and each of these lines couples into the driver through the > package > >>> inductance. The inductance of the Vss network is lumped as Lvss, and > >>> the inductance of the Vdd network as Lvdd > >>>> For a low-high transition, the > >>>> pull-up structure discharges the signal/Vdd t-line and charges the > >>>> signal/Vss t-line with ~10mA current drawn from the supply. > >>> No, a low to high transition imposes di/dt of the same polarity into > >>> both structures. The signal line is going high: It is drawing > positive > >>> convention current through the die PDN and back to the PCB PDN > through > >>> both Lvdd and Lvss. > >>> > >>>> For a > >>>> high-low transition, the the pull-down structure discharges the > >>>> signal/Vss t-line and the same 10mA from the supply charges the > >>>> signal/Vdd t-line. A constant current from the supply is steered to > >>>> charge the signal/Vss or signal/Vdd t-line. Since there is no > switched > >>>> current, di/dt is 0. > >>> No, externally current the switched current is divided in two. It is > >>> still switched. All you need to see this is to draw a black box > around > >>> the IC. What the signal line does is complemented by the PDN > lines. In > >>> order to cancel so that there is net zero current in the PDN > >>> attachments, you have to reduce the net signal current to zero, > such as > >>> trivially with differential or less trivially with an Nb(N+M)q coding > >>> scheme. > >>>> Power noise would be limited to crowbar current or a gap in > conduction > >>>> between pull-up/pull-down structures. For high performance buffer > >>>> designs, this should already be small. > >>>> > >>>> In the case of a Vss only referenced t-line, the power supply current > >>>> switches between 0-20mA resulting in SSN. > >>>> > >>>> The bus needs to be unidirectional to take full advantage of > >>>> symmetrically referenced signaling. > >>>> > >>>> Thanks, > >>>> Vinu > >>>> > > > > > -- > 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 > > > -- 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