[PCB_FORUM] Re: 0.5 mm BGA, whew!

Gene,

Thanks for the response!

-  We have almost exclusively been using DDI for fab, and yes they can do
stacked micro vias (even Top to Bottom on a 10 layer board).
-  Yes I would have the micro vias filled when in pad.
-  I guess it does make sense that you can't include the vias in the symbol,
especially when using SMVs.
-  I guess it makes sense to have the database set up as mm.  I hope the Fab
house doesn't have a problem with it.  I have not worked in a Metric design,
anything to look out for, maybe post processing?

Most, if not all, of the signals coming out of this BGA have impedance
requirements.  These signals will have to reference to a gnd or pwr plane.
The BGA balls will be either five or six rows deep, so I believe I will need
three routing layers to get out.  The way I figure it, micro vias will have
to go down to at least layer four (Top-route, L2-gnd, L3-sig, L4-sig, L5-pwr
and Bottom).  We usually like to not have signal to signal, so going to an
eight layer puts the second inner route layer at L6 (SMVs down to this
layer).

Am I missing something, or are SMVs down to L4 the only way to get impedance
critical lines out of a five ball deep 0.5 mm BGA?

Thanks again Gene!
Gary E. MacIndoe
PCB Design Engineer
Advanced Micro Devices, Inc.
Longmont, Colorado


  -----Original Message-----
  From: Gene Carman [mailto:gcarman@xxxxxxxxxxxxxxx]
  Sent: Friday, October 29, 2004 10:28 AM
  To: icu-pcb-forum@xxxxxxxxxxxxx
  Subject: [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: