In order to increase the reliability
of the converter design using the TPS7H500x-SP series, the following layout
guidelines should be followed.
- Route the feedback trace as
far away as possible from power magnetics components (inductor and/or power
transformer) and other noise inducting traces on the printed circuit board
(PCB) such as the switch node. If the feedback trace is routed beneath the
power magnetic component, ensure that this trace is on another layer of the
PCB with at least one ground layer separating the trace from the inductor or
transformer.
- Minimize the copper area of
the converter switch node for the best noise performance and reduction of
parasitic capacitance to reduce switching losses. Ensure that any noise
sensitive signals, such as the feedback trace, are routed away from this
node as it contains a high dv/dt switching signal.
- All high di/dt and dv/dt
switching loops in the power stage should have the paths minimized. This
will help to reduce EMI, lower stresses on the power devices, and reduce any
noise coupling into the control loop.
- Keep the analog ground of the
controller (AVSS) separate from the power ground of the power stage that
contains high frequency, high di/dt currents. These two grounds should be
connected at a single point in the PCB layout. The sources of power
semiconductor switches, the returns for bulk input capacitors of the power
stage, and the ouput capacitor return should all be connected to the PCB
power ground.
- All high current traces on
the PCB should be short, direct, and as wide as possible. A good rule is to
make the traces a minimum of 15 mils (0.381 mm) per ampere.
- Place all filtering and
bypass capacitors for VIN, REFCAP, and VLDO as close as possible to the
controller. Surface mount ceramic capacitors with lower ESR and ESL are
recommended as these reduce the potential for noise coupling compared to
through-hole capacitors. Care should be taken to minimize the loop area
formed by the bypass capacitor connection, the respective pin, and AVSS.
Each bypass capacitor should have a good, low impedance connection to
AVSS.
- External compensation
components should be placed near the COMP pin of the controller. Surface
mount components are recommended here as well.
- Attempt to keep the resistor
divider used to generate the voltage at VSENSE close to the device in order
to reduce noise coupling. Minimize stray capacitance to the VSENSE pin.
- OUTA, OUTB, SRA, and SRB are
used to drive the inputs of a gate driver, isolator, or gate drive
transformer. The PCB traces connected to these pins carry high dv/dt
signals. Reduce noise coupling by routing these these PCB traces away from
any traces connected to VSENSE, COMP, RT, CS_ILIM, HICC, LEB, RSC, PS, and
SP.
- In addition to utilizing the
leading edge blank time programmability of the controller, RC filtering may
be required for the sensed current signal input to CS_ILIM. Keep the
resistor and capacitor in close vicinity to CS_LIM to filter any ringing
and/or spikes that may be present on the sensed current signal.
- When operating in internal
oscillator mode with SYNC as an output, route the SYNC signal away from
noise sensitive signals/pins such as VSENSE, COMP, RT, CS_ILIM, LEB, RSC,
PS, and SP. Special care should be taken to eliminate noise from SYNC to
HICC since these pins are adjacent to one another. It is recommended that
the capacitor from HICC to AVSS be at least 3.3 nF to help with the
reduction of the noise.
- For CFP option, connect the
backside metallization of the TPS7H500x-SP to the AVSS plane of the PCB
using multiple vias. It is recommended to avoid putting solder paste
directly on top of the vias unless these vias are tented or filled.