[SI-LIST] Re: BGA Breakout.

I avoid this assembly problem (solder wicking away from the mounting pad)
by covering the pad on the BGA side with soldermask and plugging the via on
the top side.  Works great. 

On the reverse side, I leave the pads exposed to facilitate testing.

Lee


> [Original Message]
> From: Sol Tatlow <Sol.Tatlow@xxxxxxxxxxxxxxxxxxxx>
> To: <si-list@xxxxxxxxxxxxx>
> Cc: Robert Szumowicz <robert.szumowicz@xxxxxxxxxx>
> Date: 1/21/2010 9:00:13 AM
> Subject: [SI-LIST] Re: BGA Breakout.
>
> Suresh,
> One word of warning: this method can work well - it can be a good
> compromise to achieve more affordable boards - BUT you must be sure that
> either a) the vias are completely covered on the BGA side, or b) that
> there is at least approximately 0,1mm+ solder mask between BGA pad and
> via. These are basic requirements for breaking out any BGA but they are
> even more important if using this method.
>
> I mention this because you can otherwise produce assembly problems under
> the BGA with the "off-grid" positioning of the vias that you will only
> come across once the PCBs are manufactured (possibly even only once they
> are assembled): either direct shorts from BGA pads to vias on other
> nets, or open connections where the solder paste/ball has run from the
> pad into the via.
>
> By the way: in addition to the general reason for employing this
> 'trick', it can also be used on boards with 0,1mm traces for diff pairs
> - that is, if the stack-up is arranged so as to give ~50 Ohms for 0,1mm
> traces, you will have to go a little thinner to get 100 ohm for a diff
> pair (~0,08mm... and YES, this trace-width is still manufacturable with
> good yields at volume, depending upon manufacturer and other factors),
> but the spacing must also be increased, so that the resulting track-gap
> requirements don't quite fit to the 0,5mm space between 0,5mm vias on a
> 1mm pitch...
>
> Sol
>
>
> Robert Szumowicz schrieb:
> > Suresh,
> > the ASCII picture shows (I hope) the idea of via pattern giving some 
> > extra routing space:
> >
> >
> >                    1         2         1
> >                   trace    traces     trace
> >               .-.  |  .-.  |  |  .-. |  .-.    [....]
> >               '-'  |  '-'  |  |  '-' |  '-'
> > 1 trace       ----         |  |      |
> >               .-.     .-.        .-.    .-.
> >               '-'     '-'        '-'    '-'
> >               ---------
> > 2 traces      ---------
> >               .-.     .-.        .-.    .-.
> >               '-'     '-'        '-'    '-'
> > 1 trace       ---------
> >               .-.     .-.        .-.    .-.
> >               '-'     '-'        '-'    '-'
> >               ---------
> > 2 traces      ---------
> >               .-.     .-.        .-.    .-.
> >               '-'     '-'        '-'    '-'
> > 1 trace       --------
> >               .-.     .-.        .-.    .-.
> >               '-'     '-'        '-'    '-'
> >
> >              [...]
> >
> > Robert
> >
> > Suresh Kumar - ERS, HCL Tech wrote:
> >   
> >> Hi Robert,
> >>
> >> That's very interesting!
> >>
> >> I am find my imagination not working to visualize the " two traces
between 
> >> every second routing channel "
> >>
> >> so, Could you pl. send me some snap shot to understand better  ?
> >>
> >>
> >> thanks in advance
> >>
> >> regards,
> >> Suresh
> >>
> >>
> >> -----Original Message-----
> >> From: si-list-bounce@xxxxxxxxxxxxx
[mailto:si-list-bounce@xxxxxxxxxxxxx] On Behalf Of Robert Szumowicz
> >> Sent: Thursday, January 21, 2010 3:01 PM
> >> To: si-list@xxxxxxxxxxxxx
> >> Subject: [SI-LIST] Re: BGA Breakout.
> >>
> >> I have designed boards where 2 traces are routed between 1mm BGA vias 
> >> without going for very thin traces/clearances or small drills (for me
it 
> >> meant 0.125mm trace/clearance and 0.25mm/0.5mm vias). I used a trick 
> >> with a non regular via pattern what allowed routing two traces between 
> >> every second routing channel (not two traces in-between all vias). As
a 
> >> result ~30% more traces can escape a BGA per an internal signal layer.
> >>
> >> Non regular via patter which I invented meant that vias were not
centred 
> >> between four BGA pads but rather placed with an varying offset to
build 
> >> an extra horizontal and vertical routing channels.
> >>
> >> Robert
> >>
> >>
> >> Lee Ritchey wrote:
> >>   
> >>     
> >>> 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:
> >>>>>>> http://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:     
> >>>>>>>         http://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:
> >>>>>> http://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:     
> >>>>>>                http://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:
> >>>>> http://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:     
> >>>>>                 http://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:
> >>>> http://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:     
> >>>>          http://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:
> >>> http://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:     
> >>>           http://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:
> >> http://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:     
> >>            http://www.freelists.org/archives/si-list
> >>  
> >> Old (prior to June 6, 2001) list archives are viewable at:
> >>            http://www.qsl.net/wb6tpu
> >>   
> >>
> >>
> >>
> >> DISCLAIMER:
> >>
----------------------------------------------------------------------------
-------------------------------------------
> >>
> >> The contents of this e-mail and any attachment(s) are confidential and
intended for the named recipient(s) only. 
> >> It shall not attach any liability on the originator or HCL or its
affiliates. Any views or opinions presented in 
> >> this email are solely those of the author and may not necessarily
reflect the opinions of HCL or its affiliates. 
> >> Any form of reproduction, dissemination, copying, disclosure,
modification, distribution and / or publication of 
> >> this message without the prior written consent of the author of this
e-mail is strictly prohibited. If you have 
> >> received this email in error please delete it and notify the sender
immediately. Before opening any mail and 
> >> attachments please check them for viruses and defect.
> >>
> >>
----------------------------------------------------------------------------
-------------------------------------------
> >>   
> >>     
> >
> >
> > ------------------------------------------------------------------
> > 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:
> > http://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:     
> >             http://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:
> http://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:     
>               http://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:
http://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:     
                http://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: