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