Issue link: https://resources.pcb.cadence.com/i/1541046
18. Optimizing Regulator and Power Converter Current Loops How To Implement 1. Study the IC datasheet layout recommendations: f Locate the "PCB Layout Guidelines" section - nearly all power IC datasheets will illustrate and emphasize critical current paths. f Identify which pins connect to VIN, VOUT, SW (switch node), GND, PGND, EN, and FB (feedback), and note which capacitors or inductors should be closest to which pins. 2. Place input and output capacitors for the smallest loop area: f Place the input cap (often a low-ESR ceramic, e.g., 10-22 µF X7R) as close as possible to both the VIN pin and the regulator's ground return pin (PGND). f Keep traces short, thick, and wide (minimum 20-40 mil for several amps; thicker for higher currents), avoiding vias if possible. 3. Optimize switch node (SW) geometry and isolation: f Minimize the copper area of the switch node (SW) itself to reduce radiated fields but make it wide enough to carry the peak current with acceptable heating. f Avoid routing any signal, analog, or low-level traces under or near the SW node. 4. Cluster catch diode, inductor, and output cap: f Place the output inductor and catch diode (if needed) as close as possible to the SW node. f Position the output capacitor adjacent to the inductor and connect directly to the output power and ground return (shortest possible loop). f For synchronous regulators, place both high-side and low-side FETs close together to minimize loop area. 5. Separate high-frequency and low-frequency grounds: f If the IC has both AGND and PGND (analog/digital and power grounds), follow the vendor's recommendation to join these at a single point under or near the IC (star point), with a solid ground plane beneath. 6. Connect feedback and sense traces away from noisy nodes: f Route feedback (FB) and voltage sense traces away from the SW node and high-current paths; use Kelvin connections to the output capacitor ground side if possible. f Shield FB lines with a ground pour or trace to prevent noise pickup. 7. Thermal and EMI considerations: f Add a ground copper pour under the IC and power components for heat spreading; tie to the ground plane with multiple vias. f For EMI, add a guard ring or ground "fence" around the power block, stitched with vias. 8. Review and iterate: f Simulate or check loop inductance if possible; re-check with EMI pre-compliance or scope probes during prototype bring-up. f Review with your SI/PI or EMC engineer before finalizing. Common Pitfalls, Their Impact, and How to Avoid Them Common Pitfall How to Avoid it Placing caps or inductors too far from the IC Increases loop area, switching spikes, and EMI – Place them as close as possible and on the same side of the board to keep traces short. Routing FB (feedback) or analog sense lines near SW (switch node) or power paths Injects noise into the feedback, causing insta- bility or oscillation – Route perpendicular to power traces and use ground planes to provide a low-impedance return path. Using thin traces for high-current paths Causes IR drop, excessive heating, and unpre- dictable performance – Use wider traces and/ or dedicated power planes. Neglecting thermal relief and vias Poor grounding or heat sinking can cause thermal runaway or component failure – Configure thermal relief parameters within your design and add where necessary.