That's correct.  You'll want to find a vendor who will do an 8 mil drill
in a 14mil pad.  Happy Holden is correct that this would be nasty to
fill if the hole aspect ratio is real high, but you might be able to cut
the board thickness to 30mils or less.  Finding a vendor who can put a
10 mil hole in a 14 mil pad is also possible, but you will probably have
to accept minor breakout.  Since you're filling and capping anyway,
that's not a big deal.  As long as the vendor caps off the via from the
side the BGA mounts on, things should work out with a 30mil board
thickness.

If you HAVE to go to blind vias, they don't necessarily have to be
laser drilled.  Have the board assembled with core layers on the
outsides.  If they are relatively thin cores (<4mil), and the prepreg
layer is not too thin (>=4mil), then the vias will fill naturally.  Even
lower end board shops can do this reliably.

You'll also have to think about mask defined pads, another subject
everyone likes to fight about.  If the quantities are low, don't worry
too much about it--just force your supplier to get the mask targeting
within 2mils and the opening size within 1mil and use the mask defined
pads, but if you are in the high quantity/low cost market, it's a big
deal because "standard" volume shops typically can't target the mask
that well.

Wayne Thayer

>>> [log in to unmask] 6/22/2006 6:05:33 pm >>>
I should be able to make the pads 14.65mils wide at 0.5mm spacing to
keep a
5mil pad-to-pad spacing right?

  _____

From: TechNet [mailto:[log in to unmask]] On Behalf Of Happy Holden
Sent: Thursday, June 22, 2006 1:35 PM
To: [log in to unmask]
Subject: Re: [TN] via-in-pad design



Hi Ken,
A 0.5 mm uBGA usually has ball and pad sizes of 0.175 mm to 0.3 mm
(0.007-0.012").  Normal mechanical drilling is FHS + 0.010".  Even a 6
mil
FHS leaves you with a 0.016" pad (0.41 mm) and this is usually to large
for
a 0.5 mm uBGA and the spacing would be less than 0.094mm (0.0037").
This,
on top of the fact that filling a 6 mil through-hole is near
impossible.  I
think that you have to go back and convince the customer that
laser-drilled
blind vias is the only COST-EFFECTIVE way to do 0.5 mm uBGAs.
 If they have had a problem with reliability of laser-drilled holes in
the
past - - that is another story!  There are plenty of PCB Fabricators
that do
an excellent job with laser drilling - then there are others that do
not do
a good job.  If you need a list of the top HDI fabricators, send me an
email
and I will send you a list back, as well as references for reliability
data
on laser blind vias that shows they are much more reliable than normal
through-holes (WHEN PROPERLY BUILT!).

Happy Holden
Asian Pacific Services








kwood716 <[log in to unmask]>
Sent by: TechNet <[log in to unmask]>


06/21/2006 04:04 PM


Please respond to
TechNet E-Mail Forum <[log in to unmask]>; Please respond to
kwood716 <[log in to unmask]>



To
[log in to unmask]

cc

Subject
[TN] via-in-pad design






Hi all,
I have a PCB that uses a BRF6150 uBGA (0.5mm pitch) that I need to
redesign.
The current design uses very small blind and buried vias
and the customer want to use through-all vias. The only way I can do
this is
by utilizing a via-in-pad method. Is that still
a good option? maybe used with a via-fill goo?
Thanks
Ken

 _____


Saturn PCB Design
Kenneth J. Wood CID
2737 Bishop Lane
Deltona, Fl 32725
Phone: 407-340-2668
email:  <mailto:[log in to unmask]> [log in to unmask]


---------------------------------------------------
Technet Mail List provided as a service by IPC using LISTSERV 1.8e
To unsubscribe, send a message to [log in to unmask] with following text
in
the BODY (NOT the subject field): SIGNOFF Technet
To temporarily halt or (re-start) delivery of Technet send e-mail to
[log in to unmask]: SET Technet NOMAIL or (MAIL)
To receive ONE mailing per day of all the posts: send e-mail to
[log in to unmask]: SET Technet Digest
Search the archives of previous posts at:
http://listserv.ipc.org/archives
Please visit IPC web site
http://www.ipc.org/contentpage.asp?Pageid=4.3.16
for additional information, or contact Keach Sasamori at [log in to unmask]
or
847-615-7100 ext.2815
-----------------------------------------------------



---------------------------------------------------
Technet Mail List provided as a service by IPC using LISTSERV 1.8e
To unsubscribe, send a message to [log in to unmask] with following text
in
the BODY (NOT the subject field): SIGNOFF Technet
To temporarily halt or (re-start) delivery of Technet send e-mail to
[log in to unmask]: SET Technet NOMAIL or (MAIL)
To receive ONE mailing per day of all the posts: send e-mail to
[log in to unmask]: SET Technet Digest
Search the archives of previous posts at:
http://listserv.ipc.org/archives
Please visit IPC web site
http://www.ipc.org/contentpage.asp?Pageid=4.3.16 for additional
information, or contact Keach Sasamori at [log in to unmask] or 847-615-7100
ext.2815
-----------------------------------------------------

---------------------------------------------------
Technet Mail List provided as a service by IPC using LISTSERV 1.8e
To unsubscribe, send a message to [log in to unmask] with following text in
the BODY (NOT the subject field): SIGNOFF Technet
To temporarily halt or (re-start) delivery of Technet send e-mail to [log in to unmask]: SET Technet NOMAIL or (MAIL)
To receive ONE mailing per day of all the posts: send e-mail to [log in to unmask]: SET Technet Digest
Search the archives of previous posts at: http://listserv.ipc.org/archives
Please visit IPC web site http://www.ipc.org/contentpage.asp?Pageid=4.3.16 for additional information, or contact Keach Sasamori at [log in to unmask] or 847-615-7100 ext.2815
-----------------------------------------------------