Hi Darcy,
Here is my take on your questions. I haven't actually used this
technology yet but I believe a few others here have. You may very well hear
from them as well.
1) Sure 3mil traces and spaces are do-able by some specialty shops but I
would sooner put fanout vias between the pads and route out on another layer
using more reasonable 4/4mil or larger routing. 3/3mil will just get you stuck
in a high tech board fab issue with other associated failures because of the
tiny Cu topology.
2) Yes! It actually is used when referring to both (rightly or wrongly),
so further detail is needed to be sure you differentiate between the two. It
can also describe small diameter vias in the pad with no fill. There they rely
on the minimum diameter and reflowed solder viscosity to stop solder wicking
away from the pad.
3) Yes there definitely are limits so a conversation with the target
fabricator would be in order. Some are limited to very thin single layers but
some are doing 2 layers, maybe 3 thin layers. It is not the same as regular
vias though so make sure you get the full technical scoop from the target
fabricator.
4) The talk with the fabricator is also in order for this question. Don't
forget though that your first row out doesn't need any clearances and that a
number of your internal row pads could use regular via technology. Therefore
greatly reducing the number of routes requiring clearances on the first
internal layer. Don't forget to look eagerly for any unused pins as well,
utilizing those spots for additional routing room or fewer vias required.
Sincerely,
Brad Velander
Senior PCB Designer
Northern Airborne Technology
#14 - 1925 Kirschner Road,
Kelowna, BC, V1Y 4N7.
tel (250) 763-2232 ext. 225
fax (250) 762-3374
-----Original Message-----
From: Darcy Davis [mailto:[EMAIL PROTECTED]
Sent: Thursday, October 19, 2006 4:12 PM
To: PEDA ([email protected])
Subject: [PEDA] Suggestions on BGA layout
Hey folks,
We're about to delve into our first design with a real BGA. I've certainly
been able to find a few helpful documents online, but I thought I'd run a
couple questions past this knowledge base. The part is an 84 pin VFBGA with
a ball dia. of 0.3mm (nominal) and a pitch of 0.5mm (~20mil). The array is
10x10 with a 4x4 area in the center with no balls (this leaves three "rows"
of pads around the outside of the component). We're trying to balance the
cost of new PCB technologies with the risk of poor solder joints, so I'm
looking for some recommendations.
Just so you know where we're coming from, we're currently doing 2-4layer
boards with 10/26mil vias and 4/4mil trace/space. We do most designs with
0.062" FR4, but have done 20, 30 and 40mil thicknesses as well. No laser
drilled or blind/buried vias.
1) The manufacturer recommends a 260u pad (~10mil), leaving a gap of 240u
(~9mil) between pads. For fanout, we're considering doing 3 mil traces with
a 3 mil spacing. Is this reasonable? Will this technology likely be less
expensive then microvias or other fanout alternatives?
2) Does "via-in-pad" refer to a microvia within a pad? or does it
specifically refer to a via that has been plugged to prevent solder wicking?
I assume they can plug using a conductive material as opposed to epoxy? Is
it reasonable to assume that this isn't applicable to our part since
microvias don't need plugging and conventionally drilled vias would be too
big?
3) Could we put a microvia all the way through a 2-layer 40mil PCB? 60 mil?
or is their a limit to the thickness one can laser drill? (Therefore
limiting its use to 4-layer boards only).
4) The mfgr recomends "via-in-pad" as a preference to routing out on the top
layer. What size of annular ring is necessary on the inner layer for a
microvia? If the inner layer pad has to be 10 mil, we're still limited to
3/3mil trace/space to get the middle row of signals out. Sounds like an
expensive endeavor when you account for microvias and 3/3mil traces.
Hmm. That should at least get me going. Has anybody got a fanout of a
similar BGA that they would be willing to share? I'm just really shakey on
the "right" way to fanout a BGA using micro/blind/buried vias. Thanks in
advance.
Darcy Davis
____________________________________________________________
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]
