Printed-Circuit Board Layout Guideline
www.ti.com
3
Printed-Circuit Board Layout Guideline
1. To obtain optimal performance, the power input capacitors, connected from the PMID input to PGND,
must be placed as close as possible to the IC.
2. Place 4.7-µF input capacitor as close to PMID pin and PGND pin as possible to make the high-
frequency current loop area as small as possible. Place 1-µF input capacitor GNDs as close to the
respective PMID capacitor GND and PGND pins as possible to minimize the ground difference
between the input and PMID.
3. The local bypass capacitor from CS+ to GND must be connected between the CS+ pin and PGND of
the IC. The intent is to minimize the current path loop area from the SW pin through the LC filter and
back to the PGND pin.
4. Place all decoupling capacitors close to their respective IC pins and as close as possible to PGND (do
not place components such that routing interrupts power stage currents). All small control signals must
be routed away from the high-current paths.
5. The PCB must have a ground plane (return) connected directly to the return of all components through
vias (two vias per capacitor for power-stage capacitors, one via per capacitor for small-signal
components). It is also recommended to put vias inside the PGND pads for the IC, if possible. A star
ground design approach is typically used to keep circuit block currents isolated (high-power/low-power
small-signal) which reduces noise-coupling and ground-bounce issues. A single ground plane for this
design gives good results. With this small layout and a single ground plane, no ground-bounce issue
exists, and having the components segregated minimizes coupling between signals.
6. The high-current charge paths into IN, USB, BAT, and from the SW pins must be sized appropriately
for the maximum charge current in order to avoid voltage drops in these traces. The PGND pins must
be connected to the ground plane to return current through the internal low-side FET.
7. For high-current applications, the balls for the power paths must be connected to as much copper in
the board as possible. This allows better thermal performance because the board conducts heat away
from the IC.
10
bq24187 Evaluation Module User's Guide
SLUUAI5 – April 2014
Submit Documentation Feedback
Copyright © 2014, Texas Instruments Incorporated
