The UCC12051-Q1 integrated isolated power solution
simplifies system design and reduces board area usage. Proper PCB layout is
important in order to achieve optimum performance. Here is a list of
- Place decoupling capacitors as close as possible to the device pins. For the input supply, place the capacitor(s) between pin 3 (VINP) and pin 2 (GNDP). For the isolated output supply, place the capacitor(s) between pin 14 (VISO) and pin 15 (GNDS). This location is of particular importance to the input decoupling capacitor, because this capacitor supplies the transient current associated with the fast switching waveforms of the power drive circuits.
- Because the device does not have a thermal pad for heat-sinking, the device dissipates heat through the respective GND pins. Ensure that enough copper (preferably a connection to the ground plane) is present on all GNDP and GNDS pins for best heat-sinking.
- If space and layer count allow, it is also recommended to connect the VINP, GNDP, VISO and GNDS pins to internal ground or power planes through multiple vias of adequate size. Alternatively, make traces for these nets as wide as possible to minimize losses.
- TI also recommends grounding the no-connect pins (NC) to their respective ground planes. For pins 6, 7, and 8, connect to GNDP. For pins 10, 11, and 12, connect to GNDS. This will allow more continuous ground planes and larger thermal mass for heat-sinking.
- A minimum of four layers is recommended to accomplish a low-EMI PCB design. Inner layers can be spaced closer than outer layers and used to create a high-frequency bypass capacitor between GNDP and GNDS to reduce radiated emissions. Ensure proper spacing, both inter-layer and layer-to-layer, is implemented to avoid reducing isolation capabilities. These spacings will vary based on the printed circuit board construction parameters, such as dielectric material and thickness.
- Pay close attention to the spacing between primary ground plane (GNDP) and secondary ground plane (GNDS) on the PCB outer layers. The effective creepage and or clearance of the system will be reduced if the two ground planes have a lower spacing than that of the device package.
- To ensure isolation performance between the
primary and secondary side, avoid placing any PCB
traces or copper below the UCC12051-Q1 device on
the outer copper layers.