This is a CSP package, apparently.
I would talk to the manufacturing folks. They may choose not to use
solder paste on this BGA. A device like this, whether it has 63/37 or
SAC solder balls, would be better off being reflowed without adding any
solder paste. The apertures would be left off of the stencil, and as
such should not be in the SMT pad artwork for the stencil. It would
probably be better to brush on or spray (ultrasonically) a very thin
coat of water-soluble tacky flux to the area prior to assembly, and
place the component directly onto its pads and then reflow it with the
rest of the components. This way you can use a slightly smaller pad
diameter because the small stencil aperture size is not an issue. I
would leave all of the soldermask out of the BGA pad area altogether if
you are indeed using VIP, as there are no thieving issues created by the
lack of soldermask. This way the mask registration issues will not be a
problem. You will have much more reliable solder joints without the
soldermask-defined pads.
If it is elected to use solder paste then only a type 4 or type 5
solderpaste will print repeatedly through apertures this small. However,
using a type 4 or smaller particle size solder paste requires
manufacturing process controls most assembly lines are not capable of to
prevent extraneous solder fines and other issues. You cannot just switch
pastes. The minimum clearance between soldermask opening and the edge of
the pad needs to be tightly controlled during board fabrication, print
registration needs to be tightened up, stencil aperture sizes reduced
slightly, placement pressure minimized, etc.
Wayne is correct about the overetching. It is very difficult to control
on pads this small. There are some board fabricators who do this very
well, however. Seek and ye shall find.
The other issue you need to watch: pads smaller than .015" diameter
become more and more likely to come off due to the correspondingly
smaller amounts of adhesive used to bond the copper to the laminate and
the quality of the copper lamination. Larger copper features are more
forgiving of the copper laminating process. Again, the board fabricator
must use special steps/methods for PWBs of this type. I have seen boards
with very small pads have their pads literally float up into the solder
ball during initial reflow, and further problems occurred when
attempting to rework a BGA of this type.
However, with the proper pad/soldermask design, and with the proper
fabrication steps, the design can be very robust from a manufacturing
standpoint, and very reliable in durability.
-----Original Message-----
From: TechNet [mailto:[log in to unmask]] On Behalf Of Wayne Thayer
Sent: Thursday, March 01, 2007 9:06 PM
To: [log in to unmask]
Subject: Re: [TN] BGA footprint
The pad size is the easy one!
If it's a dense 0.5mm pitch, that's equivalent to 19.7 mils. If you
need to route between pads, then you will need to use 3x3 mil
linexspace. That leaves 10.7mils for the pad. This is about 0.26mm,
and going less than that can be pretty problematic: It's hard to get
solder paste to print a dot even that small.
What that doesn't tell you is:
-For many etching technologies, the smaller the radius of curvature
(smaller round pad), the more over-etched they end up. So your 10.7 mil
pad will probably over-etch unless the pcb fab makes a special effort to
add extra "swell" to them. I have tried some flip chips with 8mil
(0.2mm) pads and seen them so over-etched they were useless.
-You need to figure out how to get a useable solder mask put on the
board. If you don't have routes between the pads, then this isn't a big
problem, but if you do, then you will need to work very carefully with
the pcb fab and you need to be prepared to reject the boards based on
poor mask alignment. You can also enter the great debate on whether to
use mask defined pads!
Wayne Thayer
>>> [log in to unmask] >>>
Hi
I am working on a new board with a 0.5mm pitch BGA and I am wonder if
someone can advise me on the footprint.
1) the datasheet says the solder ball is 0.3mm +/-0.05mm
2) IPC recommends to use 80% of ball diameter for the pad which would be
0.24mm
3) Would it be OK to use a 0.2mm pad? I am hesitant to go against
recommended size without some corroborating documentation. The reason I
would want to use 0.2mm pad is to avoid using via-in-pad.
I am curious if IPC defines footprints based on what is good for
manufacturing or is it simply theoretical?
Thanks
Bob
---------------------------------------------------
Technet Mail List provided as a service by IPC using LISTSERV 15.0 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 15.0 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 15.0
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
-----------------------------------------------------
|
