Datasheet
DSBGA Package Assembly and Use
www.ti.com
8 DSBGA Package Assembly and Use
Use of the DSBGA package requires specialized board layout, precision mounting and careful re-flow
techniques, as detailed in AN-1112 DSBGA Wafer Level Chip Scale Package (SNVA009). Refer to the
section Surface Mount Assembly Considerations. For best results in assembly, alignment ordinals on the
PC board should be used to facilitate placement of the device. The pad style used with DSBGA package
must be the NSMD (Non-Solder Mask Defined) type. This means that the solder-mask opening is larger
than the pad size. This prevents a lip that otherwise forms if the solder-mask and pad overlap, from
holding the device off the surface of the board and interfering with mounting.
The 6-bump package used for LM3691 has 300–micron solder balls and requires 10.82 mils pads for
mounting on the circuit board. The trace to each pad should enter the pad with a 90° entry angle to
prevent debris from being caught in deep corners. Initially, the trace to each pad should be 7 mil wide, for
a section approximately 7 mil long or longer, as a thermal relief. Then each trace should neck up or down
to its optimal width. The important criteria is symmetry. This ensures the solder bumps on the LM3691 re-
flow evenly and that the device solders level to the board. In particular, special attention must be paid to
the pads for bumps A2 and C2, because GND and V
IN
are typically connected to large copper planes.
The DSBGA package is optimized for the smallest possible size in applications with red or infrared opaque
cases. Because the DSBGA package lacks the plastic encapsulation characteristic of larger devices, it is
vulnerable to light. Backside metallization and/or epoxy coating, along with frontside shading by the
printed circuit board, reduce this sensitivity. However, the package has exposed die edges. In particular,
DSBGA devices are sensitive to light, in the red and infrared range, shining on the package’s exposed die
edges.
9 Board Layout Considerations
PC board layout is an important part of DC-DC converter design. Poor board layout can disrupt the
performance of a DC-DC converter and surrounding circuitry by contributing to EMI, ground bounce, and
resistive voltage loss in the traces. These can send erroneous signals to the DC-DC converter IC,
resulting in poor regulation or instability. Poor layout can also result in re-flow problems leading to poor
solder joints between the DSBGA package and board pads. Poor solder joints can result in erratic or
degraded performance.
Good layout for the LM3691 can be implemented by following a few simple design rules, as illustrated in
Figure 3.
1. Place the LM3691 on 10.82 mil pads. As a thermal relief, connect each pad with a 7 mil wide,
approximately 7 mil long trace, and then incrementally increase each trace to its optimal width. The
important criterion is symmetry to ensure the solder bumps re-flow evenly (see Section 8).
2. Place the LM3691, inductor and filter capacitors close together and make the traces short. The traces
between these components carry relatively high switching currents and act as antennas. Following this
rule reduces radiated noise. Special care must be given to place the input filter capacitor very close to
the V
IN
and GND pin.
3. Arrange the components so that the switching current loops curl in the same direction. During the first
half of each cycle, current flows from the input filter capacitor, through the LM3691 and inductor to the
output filter capacitor and back through ground, forming a current loop. In the second half of each
cycle, current is pulled up from ground, through the LM3691 by the inductor, to the output filter
capacitor and then back through ground, forming a second current loop. Routing these loops so the
current curls in the same direction prevents magnetic field reversal between the two half-cycles and
reduces radiated noise.
4. Connect the ground pins of the LM3691, and filter capacitors together using generous component-side
copper fill as a pseudo-ground plane. Then connect this to the ground-plane (if one is used) with
several vias. This reduces ground-plane noise by preventing the switching currents from circulating
through the ground plane. It also reduces ground bounce at the LM3691 by giving it a low-impedance
ground connection.
5. Use wide traces between the power components and for power connections to the DC-DC converter
circuit. This reduces voltage errors caused by resistive losses across the traces.
6. Route noise sensitive traces such as the voltage feedback path away from noisy traces between the
power components. The voltage feedback trace must remain close to the LM3691 circuit and should
be routed directly from FB to V
OUT
at the output capacitor and should be routed opposite to noise
4
AN-1772 LM3691 Evaluation Board SNVA312B–May 2008–Revised April 2013
Submit Documentation Feedback
Copyright © 2008–2013, Texas Instruments Incorporated