Circuit board layout and stack-up for the LVDS SERDES devices should be designed to provide low-noise power feed to the device. Good layout practice separates high-frequency or high-level inputs and outputs to minimize unwanted stray noise pickup, feedback and interference. Power system performance can be greatly improved by using thin dielectrics (2 to 4 mils) for power / ground sandwiches. This arrangement provides plane capacitance for the PCB power system with low-inductance parasitics, which has proven especially effective at high frequencies, and makes the value and placement of external bypass capacitors less critical. External bypass capacitors should include both RF ceramic and tantalum electrolytic types. RF capacitors can use values in the range of 0.01μF to 0.1μF. Tantalum capacitors can be in the range of 2.2μF to 10μF. Voltage rating of the tantalum capacitors must be at least 5× the power supply voltage being used.

Surface-mount capacitors are recommended due to smaller parasitics. When using multiple capacitors per supply pin, locate the smaller value closer to the pin. A large bulk capacitor is recommend at the point of power entry. This is typically in the 50uF to 100uF range and smooths low frequency switching noise. TI recommends connecting power and ground pins directly to the power and ground planes with bypass capacitors connected to the plane with via on both ends of the capacitor. Connecting power or ground pins to an external bypass capacitor increases the inductance of the path.

A small body size X7R chip capacitor, such as 0603, is recommended for external bypass. The small body size reduces the parasitic inductance of the capacitor. The user must pay attention to the resonance frequency of these external bypass capacitors, usually in the range of 20MHz to 30MHz. To provide effective bypassing, multiple capacitors are often used to achieve low impedance between the supply rails over the frequency of interest. At high frequency, use two vias from power and ground pins to the planes, reducing the impedance at high frequency.

Some devices provide separate power and ground pins for different portions of the circuit. This is done to isolate switching noise effects between different sections of the circuit. Separate planes on the PCB are typically not required. Pin description tables typically provide guidance on which circuit blocks are connected to which power pin pairs. In some cases, an external filter many be used to provide clean power to sensitive circuits such as PLLs.

Use at least a 4-layer board with a power and ground plane. Locate LVCMOS signals away from the LVDS lines to prevent coupling from the LVCMOS lines to the LVDS lines. Closely coupled differential lines of 100Ω are typically recommended for LVDS interconnect. The closely coupled lines help to make sure that coupled noise appears as common-mode and thus is rejected by the receivers. The tightly coupled lines also radiate less.

Termination of the LVDS interconnect is required. For point-to-point applications, termination must be located at both ends of the devices. Nominal value is 100Ω to match the differential impedance of the line. Place the resistor as close to the transmitter DOUT± outputs and receiver RIN± inputs as possible to minimize the resulting stub between the termination resistor and device.