SNVS294S November 2004 – May 2016 LM3671 , LM3671-Q1
PRODUCTION DATA.
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 device, resulting in poor regulation or instability.
Good layout for the LM3671 can be implemented by following a few simple design rules below. Refer to Figure 38 for top layer board layout.
In mobile phones, for example, a common practice is to place the DC-DC converter on one corner of the board, arrange the CMOS digital circuitry around it (because this also generates noise), and then place sensitive preamplifiers and IF stages on the diagonally opposing corner. Often, the sensitive circuitry is shielded with a metal pan and power to the circuitry is post-regulated to reduce conducted noise, using LDOs.
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 Technology (DSBGA) Assembly Considerations. For best results in assembly, alignment ordinals on the PC board must 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. See AN-1112 DSBGA Wafer Level Chip Scale Package (SNVA009) for specific instructions how to do this. The 5-pin package used for LM3671 has 300-micron solder balls and requires 10.82 mils pads for mounting on the circuit board. The trace to each pad must 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 must neck up or down to its optimal width. The important criteria is symmetry. This ensures the solder bumps on the LM3671 re-flow evenly and that the device solders level to the board. In particular, special attention must be paid to the pads for bumps A1 and A3, because VIN and GND are typically connected to large copper planes, inadequate thermal relief can result in late or inadequate re-flow of these bumps.
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 front-side 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.