1. technology and computing
2. electronic components

QFN
How to succeed the first time with
ultra-small QFN packages
By Duane Benson,
Marketing Manager,
Screaming Circuits
The package an IC uses has a very
significant effect on layout flexibility and layout can make the
difference between a great product, a product with questionable
reliability and something that just
doesn’t work— all with the same
basic circuit design.
Mobile device designers see
anything small as positive so
designing with small packages
doesn’t require much of a “sell”
for them.
On the other hand, many
industrial device designers,
unaccustomed to real-estate
restrictions, see small as a disadvantage. The QFN (quad flat
pack, no leads) along with the
micro-BGA (ball grid array) seem
to be the package of choice for
new RF and control devices.
With many of these new
parts, the opinion of the designer is moot. Small is the only
option. Despite the difficulties
involved in moving down to
parts with .5mm lead pitch that
can’t be hand assembled for the
prototype, there are a number of
advantages relating to ground
path and thermal management.
Like it or not, designers using the new RF standards, such
as 802.15.4 and the upcoming
802.11n will have to learn how
to effectively utilise these small
packages.
ZigBee example
Take a scenario that involves adding wireless into the redesign of a
distributed process monitor and
control system. The design pairs a
Texas Instruments MSP430F1232
microcontroller (MCU) and a
Freescale MC13192 based ZigBee
radio into each remote device for
more computing power, lower
power consumption and wireless
communications capability.
Figure 1: Difference between a QFM package that is floating up due to excessive solder in the centre pad area and a
second QFN that is properly assembled.
The MCU is available in
several packages, including
a QFN-32 but the radio part
only comes in a 5mm x 5mm
QFN-32 package. A PG2012TK
L-band GaAs FET switch is also
required and that part only
comes in a 1.1mm x 1.5mm
leadless minimold package.
The big volumes today are in
the mobile world so chip companies are catering to that market first by introducing products
in increasingly smaller packages
and in many cases, never releasing in larger form factors. By
using such small parts, the MCU
and radio were placed very close
to each other and both were
placed at an optimum distance
from the antenna.
Most QFN packages have
an exposed metal pad covering most of the underside of
the component. Generally, the
metal pad is used for grounding and heat management. This
puts the ground plane within
as little as a millimetre away
from the power connection as
well as all signal pads.
The silicon is directly bonded
to that centre metal pad which
greatly helps to conduct heat
away. Even if the size advantage isn’t important, the ability
to locate capacitors so close
to the signals, exercise control
over the physical distance of
the part from the antenna and
so effectively draw heat away
from the chip die gives the QFN
package a distinct appeal in
high-speed and RF designs.
QFN Float
At a recent trade show, I received a sample part in a 3 x
3 mm QFN package. While I
haven’t tried it yet, I’m pretty
sure that, like a water bug, the
part is light enough to float on a
water surface because it doesn’t
have enough weight to break
the surface tension. But, that’s
not what I’m talking about.
Like many high-speed QFN
packaged devices, the middle of
the part has an exposed metal
contact pad covering most of
the underside. The float that I’m
talking about happens when
there is too much solder paste
on the PCB for that centre pad.
Like the water bug, the QFN
doesn’t have enough mass to
sink down to the board.
On any surface mount device,
to a small extent, the height of
the solder paste deposit is proportional to the aperture in the
solder stencil opening (bigger
opening = taller deposit). With
most parts, that isn’t a problem
because either all of the pads
are big enough so that that
ratio doesn’t have a first order
impact, or because all of the
pads are the same size and will
be equally impacted.
Since the QFN centre pad is a
much larger opening in the stencil than the signal pad openings,
and the signal pad openings are
EE Times-India | October 2007 | eetindia.com
in the 10 - 20 mil or less range,
this deposit height-to-width ratio will have a first order impact.
When the opening for the
centre pad on the QFN is too
large, the solder paste deposit
in the centre may be taller than
the deposits on the small signal
pin pads. The part high-centres
and never gets the opportunity
to contact the signal pads. In
some cases, the part will tilt a
little sideways and contact some
of the signal pads but not all.
Solder Paste Stencil
Typically, the signal pads should
have a standoff height of 2 to
3 mils after assembly. If too
much solder is deposited in the
centre, the part can very easily
float up beyond that height
and prevent the signal contacts from connecting. To help
prevent this, the solder stencil
opening should be broken into
a series of smaller openings and
should cover between 50 and
75% of the pad area.
This means that when you
lay out your PCB, you need to
look carefully at the solder paste
layer for your QFN components.
If the solder paste layer in the
CAD package part library just
follows the copper pad pattern
or the solder mask opening, you
may need to customise the CAD
package part library to avoid
leading yourself into trouble.
To better illustrate the proper
way to make your solder paste
stencil for QFN parts, I went to
our back room and took a couple of photos of good and bad
solder paste stencil practices.
Figure 2, top half, illustrates
what a just about worst-case
stencil would look like. Actual
size for the part is 7 x 7 mm. Note
how much surface area that the
centre pad has compared to the
row of side cut-outs. With most
SMT components, it is standard
procedure to reduce the size
of the paste cut-out area in the
stencil. In a case like this, it is difficult to reduce it enough and
still get even paste distribution.
The proper option is to segment
to solder stencil are as shown in
the bottom half of figure 2.
If you just reduce the paste
opening aperture, providing
one smaller opening, but don’t
segment it, you may end up
with a part that is still too high
in the middle to assure good
contact on the signal pads and
is also unstable and will likely tilt
to one side. With leaded solder,
a single 50% sized opening may
work because of the wicking
properties of lead-based solder.
Since lead-free solder does not
wick as well, it is very unlikely to
work in a RoHS process. In both
cases, the most consistently reliable method is to segment the
stencil pattern.
The recommended practice
is to segment the solder paste
opening in the centre of the QFN.
The basic idea is that you distribute a lower quantity of solder
over a broader area. You reduce
your chances of high-centring
and other problems associated
with large paste areas, such as
out gassing and spattering.
This will give good solder
distribution with little chance
of high-centring or outgassing
problems. When you reduce or
segment the solder paste stencil
pattern, do not do the same with
the solder mask. Assembly works
best with an even distribution of
solder. Masking part of the pad
area will work against good even
paste distribution.
Specialised Copper Pad
Some parts, especially highfrequency parts, such as the
MC13192 ZigBee part, require a
segmented copper pad under
the QFN. If this is the case, it is
important to segment the solder paste stencil to match the
custom pad. It is fairly common practice to use a standard
full-size square opening and
assume that surface tension
will end up distributing the
solder in the right places. For
best reliability and buildability,
make sure that the openings
match your copper layer underneath the stencil openings. Be
sure that your stencil openings
only fall above the copper and
not over any solder-mask or
bare-board sections.
eetindia.com | October 2007 | EE Times-India
Figure 2: A worst-case stencil opening (top) with recommended practice (‘s’
in verb form) of segmenting the opening (bottom)]
The first run of the design
described above properly used
a segmented copper layer, but
had a full-size opening for the
stencil. Sure enough, that wide
opening allowed too much solder on the copper. The problem
was further exacerbated when
the solder migrated off of the
bare board areas and on to the
copper pad segments. Fixing
the stencil fixed the problem.
Larger opposites
With larger QFN parts, the opposite problem can occur in
the centre pad area. When the
square opening for the solder
paste stencil is fully open on a
larger part— say 10 x 10 mm
or larger— the paste squeegee may deform and actually
scoop too much of the paste
out of the opening.
This can lead to uneven paste
and solder voids. Both are potential reliability problems. The
solution is the same. Segment
the stencil opening to create an
even paste distribution.
Conclusion
The QFN form factor delivers
a number of advantages over
other SMT package form factors.
It is generally a smaller part and,
with the centre pad, can have
better grounding and thermal
properties.
These advantages are partially offset by layout and assembly
difficulties. By following a few
simple guidelines, you can use
the parts with confidence. Check
the layout guidelines in the component applications notes.
Segment your solder stencil
opening for the centre pad. Make
a custom component library for
your CAD package if you need
to. Then Design away.
Email Send inquiry