Don't know if anyone already mentioned this, but if you want something really funky, you should call www.amitec.com and ask them about their dielectric-plugged Plated Through Hole with a microvia in the middle. Last time I looked at this was in 2001, so this might be slightly out of date by now.. 2008/1/12, Loyer, Jeff <jeff.loyer@xxxxxxxxx>: > > Some thoughts, in no particular order (and targeted for High Volume > Manufacturing products). > > > * A paper you might find pertinent is "System Level Impact of > Stitching Vias and Capacitors for High-Speed Differential Links", > available as: > Electronic Components and Technology Conference, 2007. ECTC '07. > Proceedings. 57th > Publication Date: May 29 2007-June 1 2007 > On page(s): 357-36 > ISSN: 0569-5503 > ISBN: 1-4244-0985-3 > > * Keep in mind how stackup-specific any controlled impedance via > design will be. A via that appears >50 ohms in a thick, lower-layer > count board (say 100 mils, 6 layers), might well appear capacitive (< 50 > ohms) when the number of layers is increased. Plug-in cards (or desktop > boards) are often 60 mils thick, and only have 4 layers. For a server > design, you'd need different via designs for your baseboard versus > risers and/or plug-in cards. > > * Any realistic, precise via design would have to account for > manufacturing variation, giving a "family" of possible impedances, > rather than a single one. The impedance variations might be too small > to matter, but should be understood. For differential vias, for > instance, drill accuracy might play a significant role in the impedance. > > * Of course, each controlled-impedance via is only valid for a > particular layer entry/exit scheme. > > * These make controlled-impedance vias very challenging for > actual products. > > * Add to these points the real-estate a controlled-impedance via > might require (especially if you start talking about surrounding each > signal via with multiple ground vias), and I end up being very skeptical > that they are suitable for anything other than research or > low-volume/high-performance/long-leadtime/high-price products. For > designs where cost and TTM (Time-To-Market) are primary drivers, ugly > vias will continue to be necessary evils in our design. Some things > that can be done to minimize their impact (and I invite others to add to > the list): > > o Floorplan your high speed busses first, to optimize their > topology for layer transitions: > > * Minimize the number of transitions (vias) from driver to > receiver, including connectors and risers. Let your kHz or low MHz > signals jump around from layer to layer, while your GHz signals continue > on their dedicated layers. > > * When transitioning, go all the way through the board, > minimizing the stub. For multi-board designs, this can be very > challenging, but those are probably where this will be the greatest > issue, also. > > o Provide adequate ground stitching vias near transitions. > > I think applying guidelines like these, and absorbing the "hit" from the > vias that are necessary, will be more realistic than complex, 3-D via > design for most products. > > > > I'd also add my 2 cents about loosely versus tightly coupled... As you > point out, neither is without shortcomings. I do believe, however, > you'll want the two halves of a differential pair to be in close > proximity at any transitions - they'll be more "tolerant" of the > impedance discontinuity (and any other impedance discontinuities). I > would agree with your comment regarding wider trace widths being an > advantage to looser coupling, but am not aware of any degradation of > risetime from tight coupling, except perhaps if the traces are narrower. > > > > Disclaimer: > > The content of this message is my personal opinion only and although I > am an employee of Intel, the statements I make here in no way represent > Intel's position on the issue, nor am I authorized to speak on behalf of > Intel on this matter. > > > > > > Jeff Loyer > > > > -----Original Message----- > > From: si-list-bounce@xxxxxxxxxxxxx [mailto:si-list-bounce@xxxxxxxxxxxxx] > On Behalf Of Joel Brown > > Sent: Wednesday, January 09, 2008 8:30 PM > > To: wolfgang.maichen@xxxxxxxxxxxx; luant@xxxxxxxxxxx > > Cc: si-list@xxxxxxxxxxxxx; si-list-bounce@xxxxxxxxxxxxx > > Subject: [SI-LIST] Re: 50 Ohm Via? > > > > Wolfgang, > > > > Your point about how much simulation is worthwhile is well taken. > > I work for a small company and wear a lot of hats, I am not a full time > SI > > engineer. We do have some tools such as Hyperlynx and Hspice which in my > > opinion have been under utilized. I know Hyperlynx claims to have some > GHz > > via modeling capability but I am not sure how accurate it is and I don't > > think it takes the return path such as stitching vias into account. I > have > > been trying to do more simulation as time allows and learning along the > way. > > It's certainly not easy to learn multiple simulation environments and > all > > the pitfalls. I have yet to get to the point to where I can correlate > > measurements against simulations. > > > > How would I know what the prop delay through a via will be? > > > > To Chris: > > > > I have been reading several places that recommend using loosely coupled > > differential pairs, that is why I mentioned 50 ohms. I know there are > > religious beliefs about tightly coupled vs loosely coupled pairs. The > > material I read regarding loosely coupled pairs mentioned advantages > such as > > wider trace widths for a given impedance and avoiding degradation of > rise > > time caused by coupling between signals within a pair. > > > > Thanks - Joel > > > > > > -----Original Message----- > > From: si-list-bounce@xxxxxxxxxxxxx [mailto:si-list-bounce@xxxxxxxxxxxxx] > On > > Behalf Of wolfgang.maichen@xxxxxxxxxxxx > > Sent: Wednesday, January 09, 2008 7:19 PM > > To: luant@xxxxxxxxxxx > > Cc: si-list@xxxxxxxxxxxxx; si-list-bounce@xxxxxxxxxxxxx > > Subject: [SI-LIST] Re: 50 Ohm Via? > > > > As a simple rule of thumb: > > Usually not very important if the prop delay through the via is less > than > > about 1/6th of your signal rise time (you may be able to get away with > > 1/4th). Rise time is much more important than bit rate or clock > frequency. > > As to the number of vias - this can of course aggravate the problem; but > > > on the other hand, I wouldn't attempt to design a 10 Gb/s channel and > put > > in more than maybe two vias... > > > > just my 2 cents > > > > Wolfgang > > > > > > > > > > > > "Tony Luan" <luant@xxxxxxxxxxx> > > Sent by: si-list-bounce@xxxxxxxxxxxxx > > 01/09/2008 07:06 PM > > Please respond to > > luant@xxxxxxxxxxx > > > > > > To > > <si-list@xxxxxxxxxxxxx> > > cc > > > > Subject > > [SI-LIST] Re: 50 Ohm Via? > > > > > > > > > > > > > > How critical the characteristic impedance of via transition is? It > > depends on the bit rate, channel insertion loss and the number of vias > > on each channel.=20 > > > > BR > > Tony > > > > -----Original Message----- > > From: si-list-bounce@xxxxxxxxxxxxx [mailto:si-list-bounce@xxxxxxxxxxxxx] > > On Behalf Of Harry Selfridge > > Sent: Wednesday, January 09, 2008 6:50 PM > > To: 'SI LIST' > > Subject: [SI-LIST] Re: 50 Ohm Via? > > > > There was an article written about controlled impedance vias several=20 > > years ago by Thomas Neu of Texas Instruments. I haven't seen any=20 > > followup articles by anyone on the subject since. You can read Neu's=20 > > article online at: > > > > http://www.edn.com/index.asp?layout=3Darticle&articleid=3DCA324403 . > > > > Others may have experienced different results, but I've never found=20 > > controlled impedance vias to be necessary or useful. The distances=20 > > involved in a via are so short that any pretense of matching=20 > > impedance is negligible compared with other variations that you might=20 > > encounter over the full length of a signal path. One board we built=20 > > for a customer provided two signal paths, one with Neu's controlled=20 > > impedance vias, and duplicates without. Testing of the loaded board=20 > > showed no appreciable difference in performance, and the loss of=20 > > board space to the structure necessary to achieve the controlled=20 > > impedance vias was considerable. > > > > Regards - Harry > > > > At 05:51 PM 1/9/2008, you wrote: > > >Is there such a thing as a design methodology for designing a PCB via > > with > > >50 ohm impedance, or does it have to be done iteratively using a 3D > > field > > >solver? > > >Are controlled impedance vias necessary, worthwhile or helpful for > > >multi-gigabit serial links running at 1 to 5 Gbps? > > > > > > > > > > > >Thanks - Joel > > > > ------------------------------------------------------------------ > > 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: =20 > > > //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 > > =20 > > > > ------------------------------------------------------------------ > > 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 > > > ------------------------------------------------------------------ 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