LM3673

SNVS434L – JULY 2006 – REVISED OCTOBER 2015

www.ti.com

11 Layout

11.1 Layout Guidelines

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 LM3673 can be implemented by following a few simple design rules below. Refer to

Figure 28 for top layer board layout.

1. Place the LM3673, 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 VIN

and GND pins.

2. 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 LM3673 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 LM3673 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.

3. Connect the ground pins of the LM3673 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 LM3673 by giving it a low-impedance ground connection.

4. 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.

5. 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 LM3673 circuit and must be direct, but

routed opposite to noisy components. This reduces EMI radiated onto the own voltage feedback trace of the

DC-DC converter. A good approach is to route the feedback trace on another layer and to have a ground

plane between the top layer and layer on which the feedback trace is routed. For the adjustable device

option, it is also best to have the feedback dividers on the bottom layer.

6. Place noise sensitive circuitry, such as radio IF blocks, away from the DC-DC converter, CMOS digital blocks

and other noisy circuitry. Interference with noise-sensitive circuitry in the system can be reduced through

distance.

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 it is post-regulated to reduce conducted noise, using low-dropout linear regulators.

20

Submit Documentation Feedback

Copyright © 2006–2015, Texas Instruments Incorporated

Product Folder Links: LM3673