[SI-LIST] Re: BGA Breakout.

  • From: "Lee Ritchey" <leeritchey@xxxxxxxxxxxxx>
  • To: "Sol Tatlow" <Sol.Tatlow@xxxxxxxxxxxxxxxxxxxx>
  • Date: Thu, 21 Jan 2010 11:08:01 -0800

Sol,
You are right that all too many engineers don't understand the PCB fabrication 
process as they should.  The knowledge is easy to get  if one is curious. 

I am aware of a few fabricators who have sufficient process control to deliver 
reliable, repeatable 1 mm pitch PCBs  with two traces between pins, but not 
very many.  If I could confine fabrication to those few, I'd take far more 
risks or push technology harder.  Unfortunately, most engineers don't have 
access to such suppliers.  Further, in the quest for lowest price- not cost- 
designs are routinely shopped around to a host of fabricators who are often not 
on my preferred list.  I need a design that will survive in this environment as 
do most of us.  (The company I cited with the yield problems did exactly this 
in order to achieve the volumes needed to support its sales.)

Maybe I should have added this qualifier to my remarks.  

I still maintain that designs going to the bulk of fabricators will suffer 
yield or reliability problems or both if designed with two track routing and 1 
mm pitch BGAs.  That is my experience so far.

Lee


----- Original Message ----- 
From: Sol Tatlow 
To: leeritchey@xxxxxxxxxxxxx
Cc: Surita Chandani; si-list@xxxxxxxxxxxxx
Sent: 1/21/2010 6:57:54 AM 
Subject: Re: [SI-LIST] Re: BGA Breakout.


Lee,

When I decided in 2001/2002 to go for 2 traces between 1mm pitch vias, I did so 
on the basis of 10 years layouting experience, detailed knowledge of the PCB 
manufacturing process, and close contact with a small handful of high quality 
PCB manufacturers - I like to be at least 99% sure that I'm doing the right 
thing before I do it... although I recognise, even if I'm 100% sure I'm right, 
I'm still wrong sometimes (particularly in 'discussions' with my better-half 
:)!).

Nevertheless, thanks for the article - nicely written, containing much of the 
basic PCB manufacturing information that I find many layouters/engineers 
_should_ be fully aware of, but aren't. Actually, it astounds me how few people 
seem to even begin to use such resources that so many well-educated and/or 
well-informed professionals like yourself go to the effort to make freely 
available - a few minutes to google and the motivation to self-educate are all 
they really need.

Anyway, I think where we are kind of getting short-circuited :) has simply (or 
at least mostly) to do with the board thickness: based on your assumption of 
120 mil boards, I would essentially agree with everything in your article. What 
I _wouldn't_ agree with is that a 1400+ ball BGA necessarily (or even usually) 
requires 22-26+ layers, and therefore a 100+ mil board, and therefore only one 
trace between vias would be possible; that there are board thicknesses where 2 
traces between 1mm pitch vias makes no sense, or is physically impossible, 
should be clear and was never an issue for me.

As I wrote, I take measures to make sure that I don't even approach this 
thickness (where possible), exactly _because_ of the reasons you mentioned. At 
around 20 layers/2,0mm board thickness (even up to 26 layers/2,4mm), the 
problems are the same... BUT the numbers are different: a 0,2mm (8 mil) or 
0,25mm (10 mil) drill is then (depending upon exact board thickness and 
manufacturer) no problem with regards to achieving adequate plating in the 
vias. This, as I said, opens the way to 0,5mm (20 mil) via pads and 2 traces 
between the via with no risk of bad yields (provided good layouting techniques 
are employed, of course!), leading in turn to more affordable boards.

That this may mean you have to consider differential pair coupling/routing at a 
different level than just whether you can achieve a required impedance or not, 
is (or should be) a no-brainer, hence the simple and short comment in the first 
paragraph of my last mail (that it depends upon how the signals are to be 
routed). At the end of the day, not all high-ballcount BGAs require all signal 
pins to be routed differentially for 10+ GHz :).

Another possibly critical factor is the targeted production volume, for obvious 
reasons - with regards to that, you don't specify a number in your article and 
I didn't mention this in my first email. Really, it's a key question that has 
to be asked right at the beginning of any project, as I'm sure you know and 
appreciate - I think we both failed to ask this key question before 
volunteering an answer, or rather, we should have mentioned it as a qualifying 
factor.

Still, there are many other factors that could be discussed too, but the basic 
essence of my answer was and remains: I am 100% sure that it could (perhaps 
even should) easily be possible for Surita to produce a functioning and 
reliable volume-production layout for a 1400+ ball BGA running 2 traces between 
1mm pitch vias, just as the original Intel application note states. My personal 
experience confirms this, at least for me.

Although... maybe this is one of those cases where I am 100% sure I'm right, 
but I'm still wrong ;)?!

Regards,
Sol

P.S. Before 2001, I also, as Robert Szumowicz mentioned, resorted to off-grid 
vias for some years, back in the days when most people quaked in their boots at 
the idea of 0,1mm and smaller traces... actually, I thought _I_ had "invented" 
it - damn ;)!



Lee Ritchey schrieb: 
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
  
    


-- 
________________________________________

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
  

Other related posts: