[SI-LIST] Re: BGA Breakout.

  • From: alex@xxxxxxxx
  • To: "Lee Ritchey" <leeritchey@xxxxxxxxxxxxx>, si-list@xxxxxxxxxxxxx
  • Date: Wed, 20 Jan 2010 20:00:00 +0100 (CET)

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
  

Other related posts: