10.1 PCB Layout Guidelines

The following guidelines are recommended for designing the board layout for the LMH1219:

1. Choose a suitable board stack-up that supports 75-Ω single-ended trace and 100-Ω differential trace routing on the board's top layer. This is typically done with a Layer 2 ground plane reference for the 100-Ω differential traces and a second ground plane at Layer 3 reference for the 75-Ω single end traces.
2. Use single-ended uncoupled trace designed with 75-Ω impedance for signal routing to IN0+ and IN0-. The trace width is typically 8-10 mil reference to a ground plane at Layer 3.
3. Place anti-pad (ground relief) on the power and ground planes directly under the 4.7-µF AC coupling capacitor and IC landing pads to minimize parasitic capacitance. The size of the anti-pad depends on the board stack-up and can be determined by a 3-dimension electromagnetic simulation tool.
4. Use a well-designed BNC footprint to ensure the BNC's signal landing pad achieves 75-Ω characteristic impedance. BNC suppliers usually provide recommendations on BNC footprint for best results.
5. Keep trace length short between the BNC and IN0+. The trace routing for IN0+ and IN0- should be symmetrical, approximately equal lengths and equal loading.
6. Use coupled differential traces with 100-Ω impedance for signal routing to IN1±, OUT0± and OUT1±. They are usually 5-8 mil trace width reference to a ground plane at Layer 2.
7. The exposed pad EP of the package should be connected to the ground plane through an array of vias. These vias are solder-masked to avoid solder flowing into the plated-through holes during the board manufacturing process.
8. Connect each supply pin (VDD_CDR, VIN, VDDIO, VDD_LDO) to the power or ground planes with a short via. The via is usually placed tangent to the supply pins' landing pads with the shortest trace possible.
9. Power supply bypass capacitors should be placed close to the supply pins. They are commonly placed at the bottom layer and share the ground of the EP.