[SI-LIST] Re: BGA Breakout.

  • From: "Lee Ritchey" <leeritchey@xxxxxxxxxxxxx>
  • To: "Sol Tatlow" <Sol.Tatlow@xxxxxxxxxxxxxxxxxxxx>
  • Date: Mon, 18 Jan 2010 12:01:37 -0800

Sol,

No fight coming from this quarter.  Several times, I have had engineers
from some of the largest network equipment suppliers in my classes with
PCBs routed as you describe.   The reason they were in the class was that
their manufacturing yields were too low from excessive shorts.  The fix was
to avoid two track routing.

I did not discuss the crosstalk issues that result from such tight routing,
but they can be significant, especially with the signal edges getting below
100 pSec.




> [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
  

Other related posts: