I guess the next question on everybody's mind (on mine, anyway) becomes: What's the lead time and cost of a new interposer design for your specific pinout plus added board analysis services grasciously provided by various high speed consulting companies who built your interposer? As you need to make a call between that and doing a couple of your own prototypes, with cleverly placed probe points and decoupling options, building your own knowledge base and design rules for the PCB process you use. Lars 2007/8/21, Julian Ferry <julian.ferry@xxxxxxxxxx>: > > Scott McMorrow is presenting a webinar this Thursday on the interposer > approach that Steve mentioned. > > For anyone interested, there is still time to sign up. > > Samtec's PowerPoser(tm) Interposers Webinar is scheduled for Thursday, > August 23, 2007 at 11:00 AM EST. > > Register at: > > http://www.connectorwizard.com/Webinars.aspx > > > Julian Ferry > High Speed Engineering Manager > Samtec, Inc. > > > -----Original Message----- > From: si-list-bounce@xxxxxxxxxxxxx [mailto:si-list-bounce@xxxxxxxxxxxxx] > On Behalf Of steve weir > Sent: Monday, August 20, 2007 4:31 PM > To: write2larsj@xxxxxxxxx > Cc: si-list@xxxxxxxxxxxxx > Subject: [SI-LIST] Re: Decoupling of digital power i PCB's, how do we > avoid pole peaks in the impedance, how far up in frequency do we need low > impedance > > Lars, Peter, today you need to collect papers. In a few months Istvan > will have a couple of books out on power delivery that will hopefully > reduce the need to hunt for tidbits here and there. Istvan also has many > excellent papers on his web site. He's got a lot of the papers by people > once of SUN as well as himself, like Larry Smith and Ray Anderson. The > X2Y web site www.x2y.com has a number of decoupling / bypass papers, as > does the Teraspeed site, www.teraspeed.com from yours truly. There is > also useful information in Lee's first book, "Right the First Time". Lee > self publishes so you have to go to his web site for that > www.speedingedge.com. > > Simulators generate hallucinations that are sometimes useful and > sometimes useless. It mostly goes back to garbage in / garbage out. But > with good source data, and an understanding of what a given simulator > assumes and how it goes about its evaluation you can get useful results > from those packages. To do so, the most important information you need > to engineer a reliable power system by design is often the most > difficult to obtain: detailed information about the: package parasitics, > internal storage, real current profile, and actual voltage requirements > of the IC's that you intend to use. We can build a power system that > looks like a dead AC short on the PCB and actually end up worse off at > the die than with a higher impedance power system. I cannot emphasize > enough the importance of either obtaining the IC information from your > vendor, or deriving it through measurements. [SHAMELESS PLUG ALERT!] > This is something that we do in Teraspeed's Portland labs. For FPGA's > Samtec and Teraspeed have developed an interposer product that > essentially shrink wraps the power system for those IC's, so you don't > have to chase that rabbit down the hole. > > When it comes to implementing the power system resonances between > different MLCC capacitors is usually a low priority issue. Below about > 20MHz you can analyze it with good accuracy using any of many 1D > parallel admittance spreadsheet tools out there, including: one Istvan > offers for free on his web site, a freebie from Altera, and one you can > buy from UltraCad. Above about 20MHz the spatial effects of the > interconnect changes what your IC die sees compared to the PCB planes. > Here any number of tools are useful, including commercial products, or > free software like Fast Henry. If you have a decent model for each of > your significant ICs, and software that is at least 2D aware, then you > can reliably predict the plane and IC power delivery. But if you don't > have decent models of your IC's, your models are going to become > fantasies where it counts: resonances created by interaction of the IC > die with the PDN. This tends to happen at frequencies well below bypass > cap network to plane cavity resonance, or the loaded PCB modal > resonances. A $100,000 software tool cannot fix faulty assumptions. > > For anything that you are going to do with capacitors, mounted > inductance is the enemy from DC to daylight. More mounted inductance > translates to more parts, and higher Q in each resonance, be it between > the VRM and bulk caps, bulk caps and MLCCs, MLCCs of different values, > or MLCCs and IC die, or MLCCs and the plane cavities. If you are going > to become religious about anything to do with PDN design, battling > inductance is a worthy crusade. Multiterminal caps like X2Y(tm)'s ( I > consult to X2Y(tm) ) offer a lot of help in the battle against > inductance. An exciting recent development is that Samsung is now making > X2Y(tm) caps up to 2uF total in an 0603 package. > > So my bottom line is: Get IC data. Understand and limit resonances. > Terminate inductance with extreme prejudice. > > Good luck. > > > Steve > > Lars Juul wrote: > > Hej Peter, > > A brief comment on your last statement: > > > >> It looks like I am back in the old days where we build a prototype and > then > >> > > started to find the correct components values? > > > > Even though you can literally spend 100K's of $$$ on simulation tools > that > > can extract your board layout and simulate your decoupling network, you > > always have to make the call whether it's > > > > a) cheaper and faster to build a few prototypes, building your own set > of > > decoupling design rules based on your already good understanding of > linear > > systems. > > > > or > > > > b) preferable to come up with a simulation flow where the results are > > correllated to the boards you produce, enabling you to quickly verify > your > > layout. > > > > Either way, you need to build a knowledge base of do's and don'ts and > that > > experience doesn't come for free. > > > > a) is the choice if you're focusing mostly at perfecting one product at > a > > time, and if you or your test and measurement folks are experienced, > able to > > effectively pinpoint the defects of a design. > > > > b) is the choice if you have a steady flow of new designs coming > enabling > > you to constantly correllate your results and have fewer redesigns. The > > initial matching of simulation and measurements can be a painful, > lengthy > > affair, though. > > > > My point is, the EDA folks will always try to convince you that using > their > > tools you'll always have hole-in-one designs, but for me prototyping > remains > > as the most secure way of ensuring your board works. > > > > And I'd rather put my money on something that works in the lab rather > than > > in a simulator. > > But again, that's just my ?0.02. > > > > Best regards, > > Lars > > > > 2007/8/20, istvan novak <Istvan.Novak@xxxxxxx>: > > > >> Peter, > >> > >> A few quick answers/observations: > >> > >> 1) How far down the IC needs low impedance? > >> The core power distribution circuit from the chip's perspective is > >> probably OK with a high > >> impedance at 900MHz; the package and/or silicon has to take care of > that > >> frequency range. > >> SI and EMI may suffer though; if you happen to route signal traces > >> referencing this core > >> plane, the signal may suffer too much. Similarly, dependent on the PCB > >> and system > >> constructions, the resonance may create EMI problem. > >> > >> 2) Higher ESR capacitors; do they exist? > >> In ceramic MLCCs, they start to appear on the market. You can look at > >> the DesignCon > >> 2007 presentations at http://home.att.net/~istvan.novak/papers.html > >> > >> 3) How many of you do power impedance analyses during design? > >> Well, at large OEMs we have to do at least some sort of analysis, > >> sometimes very detailed > >> designs and validations. > >> > >> In general, the problem you notice is the resonance between the > >> inductances of the bypass > >> capacitors resonating with the static capacitance of the planes. There > >> are a few ways of > >> helping it: > >> - you can make the static capacitance lower (this pushes out the > >> resonance frequency). > >> You can lower the capacitance by placing the power/ground planes > further > >> away, but > >> this also increases the plane inductance; this is not your first > >> choice. You can. however, > >> make the plane shape as small as possible (with some boundary area > >> left), this will > >> minimise capacitance. > >> - as you pointed out, you can increase the ESR of parts. This does not > >> change the > >> resonance frequency, but reduces the peak. Dependent on what > >> mid-frequency > >> impedance you need, you can simply use R-C components with > low-inductance > >> layout, or you can consider the high-ESR MLCCs. > >> - finally, a brute force solution, not requiring special part is to > >> overwhelm the inductance > >> of the plane. If cumulatively your capacitors present an inductance, > >> which is about 1% > >> of the plane inductance, the resonance peak is mostly gone. To achieve > >> this, you can > >> place the power/ground planes close to the surface, so that via > >> inductance is less, or > >> can use multiple vias for each capacitor, use low-inductance > capacitors, > >> like reverse > >> geometry, X2Y or multi-terminal capacitors. > >> > >> Regards, > >> > >> Istvan Novak > >> SUN Microsystems > >> > >> > >> Peter Sørensen wrote: > >> > >> > >>> At present I am trying to analyse and fix the impedance of my digital > = > >>> power > >>> supplies in our new PCB construction. > >>> This turns out to be more complex than most digital designers think. > >>> I have read a number articles and a book so far, but I have not found > = > >>> the > >>> solution. It just made me able to do simulation in a spreadsheet and > >>> visualize the problem. > >>> > >>> Modern SMD capacitors have low ESR =3D high Q. They also have some = > >>> inductance, > >>> but do not forget the VIA inductance which often is bigger than the > >>> component itself. Traces are totally forbidden in my world due to > >>> inductance. Large caps like 1210 get one via on each side of the pad. > >>> These stray inductors combined with the capacity generates zeros and = > >>> poles. > >>> The zero's are great they reduce the impedance to the ESR value plus > >>> resistance in VIA's, equal to a very low impedance at some > frequencies. > >>> Using many capacitors increases the frequency area with a low > impedance. > >>> Power Planes places close to GND planes are great, they makes capacity > = > >>> with > >>> zero inductance for any frequency that matters, but they only works at > = > >>> high > >>> frequencies especially if you have small planes. > >>> > >>> I have made some simulations showing that with a small power plane of > 2 > >>> square inch (a core voltage use by one BGA) I get a huge pole at > >>> 900MHz. The impedance is above 0.05 ohms from 100MHz and up 3 GHz. The > >>> question is how far down do IC's need a low impedance. > >>> At 3 GHz is does not matter, at this frequency only decoupling in = > >>> silicium > >>> will work due to inductance in package etc. > >>> But what about the 100MHz, I believe a low impedance must be provided > = > >>> for > >>> many IC's up to about 300MHz or even more. > >>> Eg. This core is running at 400MHz and I would like a low impedance in > = > >>> that > >>> range. > >>> The IC's supplier do not specify supply impedance, many have PCB > layout > >>> guidelines but often they can not be copied. > >>> For this one I used one 1210 100uF and an array of twenty 0402 220nF. > = > >>> Adding > >>> more caps would help but there is not room. > >>> The simulation result also depends on what you estimate your via's > >>> inductance and resistante to be. > >>> > >>> What really would help would be capacitors with higher ESR =3D low Q. > = > >>> They > >>> would lower the poles impedance and raise the zero impedance. > >>> Do they exist? > >>> Properly not, I have not beeen able to find them. > >>> > >>> Using leaded components is not an option, they may have lower Q but > they > >>> will also have more inductance and use more space etc. > >>> > >>> Combining two or more values of array caps in 0402 house like 220nF+ = > >>> 10nF > >>> does not help much and generate a new pole between the two zero's, > this = > >>> poel > >>> is lower but also at a lower and more critical frequency. > >>> > >>> To me it looks impossible to garantee a low impedance of below 0.05ohms > >>> > >> = > >> > >>> or > >>> better at the intire frequency range of interest. > >>> > >>> I belive the reason that most digital designs still works is that the > = > >>> poles > >>> do not match the load frequencies in most applications. > >>> I believe most designers still do as usual and then cross their > fingers = > >>> and > >>> hope they do not have any poles at critical frequencies. > >>> How many of you do power impedance analyses during design? > >>> > >>> It looks like I am back in the old days where we build a prototype and > = > >>> then > >>> started to find the correct components values? > >>> > >>> Best regards > >>> Peter S=F8rensen > >>> > >>> > >>> > >>> > >>> > >> ------------------------------------------------------------------ > >> 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 > > > > > > > > > > > > > -- > Steve Weir > Teraspeed Consulting Group LLC > 121 North River Drive > Narragansett, RI 02882 > > California office > (408) 884-3985 Business > (707) 780-1951 Fax > > Main office > (401) 284-1827 Business > (401) 284-1840 Fax > > Oregon office > (503) 430-1065 Business > (503) 430-1285 Fax > > http://www.teraspeed.com > This e-mail contains proprietary and confidential intellectual property of > Teraspeed Consulting Group LLC > > ------------------------------------------------------------------------------------------------------ > Teraspeed(R) is the registered service mark of Teraspeed Consulting Group > LLC > > ------------------------------------------------------------------ > 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