I will have it posted on my web site www.speedingedge.com by tomorrow along with several other pertinent papers by tomorrow. It will be under "Related Articles". We will have a booth at DesignCon. Stop by and see us. That's Speeding Edge. Meantime, here is a copy for you. Lee > [Original Message] > From: <alex@xxxxxxxx> > To: Lee Ritchey <leeritchey@xxxxxxxxxxxxx>; <si-list@xxxxxxxxxxxxx> > Date: 1/20/2010 1:00:13 PM > Subject: [SI-LIST] Re: BGA Breakout. > > Hi Lee, > > Could you please put the "attached" file on a server somewhere so > everybody on the SI-LIST can check it? The server is not distributing > attachments.... > > Thank you very much, and I hope to see you at DesignCon! > > > Alexandre Desnoyers > > > > Sol, > > I have attached an analysis I did of clearances, tolerances and > > reliability > > requirements when routing PCBs. Hope this makes it clear what the risks > > are when routing 2 between on 1 mm pitch BGAs. > > > > Lee > > > > > >> [Original Message] > >> From: Sol Tatlow <Sol.Tatlow@xxxxxxxxxxxxxxxxxxxx> > >> To: Lee Ritchey <leeritchey@xxxxxxxxxxxxx> > >> Cc: Surita Chandani <surita.chandani@xxxxxxxxx>; <si-list@xxxxxxxxxxxxx> > >> Date: 1/18/2010 1:39:42 PM > >> Subject: [SI-LIST] Re: BGA Breakout. > >> > >> With all respect, Lee, I beg to differ (at least a little bit ;)!): I > >> personally have routed many boards with 1mm BGAs of over 1700 balls > >> (with 1200+ signals, ALL 1700+ balls connected), and, depending upon how > >> these signals are to be routed (which is, admittedly, a fairly big > >> 'depending'), 18 layers can be (and usually is) enough already. > >> Since roughly 2001/2002, I have had such BGAs on boards where I > >> generally have around 18-20 layers in <2,0mm (78 mil) together with > >> 0,5mm (20mil) via pads (the drill doesn't really interest me, in > >> general, just the reliability of the results!) - this leaves 0,1mm (4 > >> mil) track and gap (roughly speaking) for 2 tracks between vias... and > >> the '2 traces between the vias' is the key to holding down board > >> thickness and layer count. This has worked for me even up to 26 layers > >> and ~2,5mm board thickness. > >> > >> With (in the meantime) 30,000-60,000 component pins/balls per board, and > >> a resulting via count of only somewhat less than the pin count, it is > >> still possible to have these boards manufactured in series quantities at > >> affordable prices from a comfortable number of manufacturers around the > >> world; the results, in some cases, have been in operation since 2002 and > >> we have very good reliability results across the board (I sweated back > >> then a little, but in the meantime, it's 100% normal... I sleep easily > >> at night now :D!!). > >> > >> One typical problem occurs, of course, in the planning phase: if you > >> assume too many power/gnd _pairs_ (as opposed to _individual_ gnd or pwr > >> layers), you are automatically forced to have a thicker board, where it > >> may no longer be possible to have small enough vias to route 2 tracks > >> between the vias; this is a downward spiral, of course, forcing the > >> number of signal layers up, and then again, the pwr/gnd count. > >> > >> I have, up until now, avoided having exclusively pwr/gnd power > >> sandwiches (however nice an idea these are) for exactly this reason; > >> instead, alternating (in general) GND-SIG-SIG-PWR-SIG-SIG- etc. coupled > >> with good routing strategies has given me very good results - there are > >> many proponents for always using pwr/gnd 'sandwich' pairs, but this is, > >> quite simply, not always necessary). > >> > >> Not that I want to start a fight, Lee, just wanted to voice my > >> experience/opinion :D!! > >> > >> Regards, > >> Sol > >> > >> P.S. What 'affordable' means, depends, of course, on the end product ;), > >> but usually, the 0,1mm track and gap means reduced costs in comparison > >> to thicker boards with more coarse structures and higher layer count... > >> in some cases, you might even go to slightly bigger via pads and LESS > >> than 0,1mm track and gap, to reduce costs... this depends upon the > >> manufacturer, thickness of the board, availability of specific > >> materials, etc. > >> > >> Lee Ritchey schrieb: > >> > Surita, > >> > > >> > I believe this kind of routing is possible with very thin PCBs with > >> very > >> > small holes such as in laptop motherboards. However, with very large > > BGAs > >> > such as yours, it is unlikely that it w ill route on a thin PCB. My > >> > experience with BGAs of your size is that a 22-26 layer PCB will be > > needed > >> > and that will likely be 100+ mils thick resulting in the need for 12 > >> mil > >> > drills. > >> > > >> > Lee > >> > > >> > > >> > > >> >> [Original Message] > >> >> From: Surita Chandani <surita.chandani@xxxxxxxxx> > >> >> To: <si-list@xxxxxxxxxxxxx> > >> >> Date: 1/15/2010 11:43:41 AM > >> >> Subject: [SI-LIST] Re: BGA Breakout. > >> >> > >> >> Thanks Lee for your comments. > >> >> The suggestions for two traces between Vias comes directly from Intel > >> >> > >> > document, also this document is from 2002. Their pitch is 1.067 mm. > >> The > >> > document itself is available at: > >> > > >> >> > >> >> http://download.intel.com/support/processors/xeon/sb/25039702.pdf > >> >> ; Page 43. > >> >> > >> >> > >> >> > >> >> --- On Fri, 1/15/10, Lee Ritchey <leeritchey@xxxxxxxxxxxxx> wrote: > >> >> Surita, > >> >> > >> >> You are right, you cannot successfully route two traces between pins > > on a > >> >> > >> > 1 > >> > > >> >> mm pitch BGA without significant risk of shorts. > >> >> > >> >> If you drill a 12 mil hole, your antipad does not have to be larger > > than > >> >> > >> > 32 > >> > > >> >> mils. This leaves you with a 7.37 mil web, which works nicely for a > >> >> > >> > single > >> > > >> >> trace, but not two traces.. Your surface or signal layer pads can be > > 24 > >> >> mils for 1 mil annular ring and 26 mils for 2 mil annular ring. > >> >> > >> >> There will only be pads on inner layers where traces connect. > >> >> > >> >> By the way, what vendor told you to route 2 traces between pins? > >> >> > >> >> Lee Ritchey > >> >> > >> >> > >> >> > >> >> > >> >>> [Original Message] > >> >>> From: Surita Chandani <surita.chandani@xxxxxxxxx> > >> >>> To: <si-list@xxxxxxxxxxxxx> > >> >>> Date: 1/14/2010 9:19:08 AM > >> >>> Subject: [SI-LIST] BGA Breakout. > >> >>> > >> >>> > >> >>> > >> >>> > >> >>> Hello Gurus; > >> >>> > >> >>> > >> >>> > >> >>> I am doing some preliminary calculations on the breakout of > >> >>> a 1,400+ Ball , BGA. Roughly one half of them are signal > >> >>> connections which would need traces running up to them. The vendor > >> >>> > >> > claims > >> > > >> >> you > >> >> > >> >>> can run two traces between Vias, my calculations are not adding up, > >> I > >> >>> > >> >> have a > >> >> > >> >>> few questions. > >> >>> > >> >>> > >> >>> > >> >>> 1. Generally, do the Vias have a pad even on the signal > >> >>> layer it is not connecting to?. > >> >>> > >> >>> > >> >>> > >> >>> 2. Do the Vias have a larger pad on the inner layers? > >> >>> > >> >>> > >> >>> > >> >>> 3. With a Ball pitch > >> >>> of 1 mm (39 mils.) and an Antipad of 35 mils, there is hardly any > >> room > >> >>> > >> >> for one > >> >> > >> >>> trace between Vias, what am I doing wrong? > >> >>> > >> >>> > >> >>> > >> >>> Thanks, > >> >>> > >> >>> > >> >>> > >> >>> Surita Chandani > >> >>> > >> >>> > >> >>> > >> >>> > >> >>> > >> >>> ------------------------------------------------------------------ > >> >>> 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 > >> >>> > >> >>> 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 > >> >> > >> >> 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 > >> > > >> > Old (prior to June 6, 2001) list archives are viewable at: > >> > http://www.qsl.net/wb6tpu > >> > > >> > > >> > > >> > >> -- > >> ________________________________________ > >> > >> Sol Tatlow, M. Eng. (Oxon) > >> Product Developer > >> > >> Pro Design Electronic GmbH > >> Albert-Mayer-Str. 16 > >> D-83052 Bruckmuehl > >> Phone: +49 (0) 8062/808-302 > >> PCFax: +49 (0) 8062/808-2302 > >> sol.tatlow@xxxxxxxxxxxxxxxxxxxx > >> www.prodesign-europe.com > >> ________________________________________ > >> > >> Vertretungsberechtigte Geschaeftsfuehrer: > >> Helmut Mahr, Ulrike Angersbach, Stephan Roeslmair, Dieter Lessenich > >> > >> Registergericht: Amtsgericht Traunstein Registernummer: HRB 13 002 > >> > >> > >> > >> ------------------------------------------------------------------ > >> 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 > >> > >> 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 > > > > 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 > > 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 Old (prior to June 6, 2001) list archives are viewable at: http://www.qsl.net/wb6tpu