Hello Darcy,
For some time now, we use laserdrilled microvias in our dense boards and
have blind via's inside an SMD pad without reflow problems.
You should use buildup boards with a thin prepreg layer between the outer
and the first inner layer so the holes are not too deep (some companies go
as thin as 60 um.
I use 12mil via / 4mil hole, 6 mil trace/space, which is quite standard HDI
(no surcharge).
You can put a blind microvia inside an SC70 pad and in pads like TSSOP or
TQFP that need to be connected to GND I place two: one from Top to MidLayer1
and one from MidLayer1 to Midlayer2. That means that these pads have no
routes at all.
As far as possible, I use a 6 Layer board and use the top 3 layers for
routing components on the Top, the bottom 3 layers for routing components on
the bottom. That means there are no through holes and you keep the whole
bottom free for another circuit.
This meand I have 2 GND planes (actually made with polygones, more flexible
to make splitted areas) and connect these planes later by adding drilled
through vias on places that are free (where applicable).
So far, most of my designs are possible with 6 layers only and with a
density approaching the total component area.
Indeed, laserdrilled via's normally go one deep, you need to add a 2nd one
adjacent for the next layer and place a short route to connect them (like we
connect a pad to GND within the pad area). I know a Swiss company that laser
drills layers 2-deep, I once made a design doing that, but that was NO
success at all! The holes were wider and deeper, giving soldering problems
due to trapper air and solder loss into the hole. In all next designs I used
staggered via's. This also makes you more flexible in selecting your
supplier, resulting in better prices.
Regarding the cost, it very much depends on the shop and their capabilities.
We make specialized equipment and our quantities are in the range of 100 or
250 at the maximum (often start lower). In these qty, I have the experience
that the costs with microvias are lower because you win so much area. But
for consumer qty I think it can be quite different.
One other thing: we always use a gold surface for these boards, a gold flash
is not that expensive.
I hope this information helped you.
With best regards,
Ton
----- Original Message -----
From: "Darcy Davis" <[EMAIL PROTECTED]>
To: "PEDA (E-mail)" <[email protected]>
Sent: Monday, September 26, 2005 11:32 PM
Subject: [PEDA] Micro Vias
We're heading into new territory for us and so looking into using micro
vias. Currently we're using 10/26mil (drill/annular ring) vias, but we're
still finding that the via's are consuming too much placement room. My
understanding is that with micro vias, we can punch a hole right through a
pad and still be OK through reflow. Does anybody know otherwise? Since
micro
vias will be laser drilled (I assume), they can only go between two
adjacent
layers, right? Is there typically a specific size of hole that must be
used,
or is there just a minimum hole size requirement? Are there any other
limitations to this technology that I may not have thought of? All else
being equal, does anyone know what the cost differential would be for a
board with micro vias vs. our current 10/26mil vias?
Thanks again,
Darcy Davis
Design Engineer
=========================================================
Dynastream Innovations, Inc. Ph: (403) 932-9292 ext. 132
228 River Ave. Fax: (403) 932-6521
Cochrane, AB T4C 2C1 Web: www.dynastream.com
Canada
=========================================================
____________________________________________________________
You are subscribed to the PEDA discussion forum
To Post messages:
mailto:[email protected]
Unsubscribe and Other Options:
http://techservinc.com/mailman/listinfo/peda_techservinc.com
Browse or Search Old Archives (2001-2004):
http://www.mail-archive.com/[email protected]
Browse or Search Current Archives (2004-Current):
http://www.mail-archive.com/[email protected]
____________________________________________________________
You are subscribed to the PEDA discussion forum
To Post messages:
mailto:[email protected]
Unsubscribe and Other Options:
http://techservinc.com/mailman/listinfo/peda_techservinc.com
Browse or Search Old Archives (2001-2004):
http://www.mail-archive.com/[email protected]
Browse or Search Current Archives (2004-Current):
http://www.mail-archive.com/[email protected]
