[PCB_FORUM] Re: 0.5 mm BGA, whew!

 

-----Original Message-----
From: Gary MacIndoe [mailto:gary.macindoe@xxxxxxx]
Sent: Friday, October 29, 2004 9:06 AM
To: Allegro Forum
Subject: [PCB_FORUM] 0.5 mm BGA, whew!


All,
 
Well, it seems to be a slow day on the Forum, so I'll through out a relatively 
involved set of questions!
 
We are looking into using a 0.5 mm BGA in a very dense design, so big time HDI 
practices will come into play: micro vias (MVs), probably even stacked micro 
vias (SMVs), in order to fan out on several layers. 
 
make sure your vendor can do stacked microvias.  Not all can.  Some insist on 
staggered.  Also becareful on high current applications... use multiple 
microvias.  
 
-  would you use the micro vias in pad or not? 
 
Yes, but if you can have them filled, that is better... the dimples can 
decrease the solder available to the balls, simply because it has more area to 
fill and this can reduce the yield on the final assembly.  Also you will find 
with that .5 pitch there is hardly any other way to break the footprint out... 
depending on the arrangement of the balls.
 
   Why?  Build them into the symbol?   No... unless you are sure you are going 
to break the symbol out this way every time. 
 
-  how can you have the micro vias built into the symbol if you don't know 
which balls will go down to which layer?   So again No on building them in. 
 
-  I will make the 0.5 mm BGA Allegro symbol with the drawing units set to 
Millimeters, but would like to keep the design database set to Mils.  Is this 
the way most of you have done it?
 
No, I just work in mm.
 
-  if the symbol is set to Millimeters and the design set to Mils, this makes 
dropping the micro vias (in pad or not) after the BGA symbol is placed in the 
design tricky.  Any other way to get around this?
 
work in mm.
 
-  So, setting up blind/buried micro vias should be the same as any 
blind/buried via.  How about SMVs?  If you have a micro via set up for layers 
1-2, 2-3, 3-4, etc., how do you avoid the DRCs when you stack them (same X,Y)?
 
Not sure... this has been my complaint about using microvias and drilled vias 
in the same designs and not having rules that differentiate them.  Others say 
"it's no problem."  BTW three layers of build up is rather rare... although it 
can be done... and there is a technology called ALIVH that is all microvias, 
and supports well using stacked microvias... but again not all PWB houses can 
do this.  (Japan is the leader here)  BTW I have been using microvias (in a 
different tool) quite successfully for about 5 years know...  So while I am a 
fairly new user of Allegro and don't fully comprehend all the subtlies of the 
tool, my microvia and design experience is far greater.
 
My head is about spinning trying to comprehend all of this micro via/stacked 
micro via stuff!
 
there is a site given the other day that had some pretty good illustrations of 
microvias...  http://www.westwoodpcb.com/
 
 
 
Any help from someone that has already used a 0.5 mm BGA on a very dense design 
with stacked micro vias would be greatly appreciated!! 
 
I have a feeling we all are going to see a lot more of this.  Good luck.  
 
Gene Carman
VIA Telecom 
 
Thanks in advance,

Gary E. MacIndoe
PCB Design Engineer
Advanced Micro Devices, Inc.
Longmont, Colorado

Other related posts: