10.1 Layout Guidelines

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

TI recommends MLCC surface mount capacitors due to their smaller parasitic properties. When using multiple capacitors per supply pin, locate the smaller value closer to the pin. TI recommends a large bulk capacitor typically in the 50 μF to 100 μF range at the point of power entry, which smooths low frequency switching noise connect 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. TI recommends a small body size X7R chip capacitor, such as 0603 or 0805, for external bypass. Because a small body sized capacitor has less inductance. The user must pay attention to the resonance frequency of these external bypass capacitors, usually in the range of 20 MHz to 30 MHz. 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, it is also a common practice to 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 may be used to provide clean power to sensitive circuits such as PLLs. This device requires only one common ground plane to connect all device related ground pins.

Use at least a four 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 100 Ω are typically recommended for LVDS interconnect. The closely coupled lines help to ensure that coupled noise will appear as common mode and thus is rejected by the receivers. The tightly coupled lines also radiate less.

At least 9 thermal vias are necessary from the device center DAP to the ground plane. They connect the device ground to the PCB ground plane, as well as conduct heat from the exposed pad of the package to the PCB ground plane. More information on the WQFN package, including PCB design and manufacturing requirements, is provided in AN-1187 Leadless Leadframe Package (LLP) (AN-2198).

Stencil parameters such as aperture area ratio and the fabrication process have a significant impact on paste deposition. Inspection of the stencil prior to placement of the WQFN package is highly recommended to improve board assembly yields. If the via and aperture openings are not carefully monitored, the solder may flow unevenly through the DAP. Stencil parameters for aperture opening and via locations are shown below:

Figure 42 shows the PCB layout example derived from the layout design of the DS90UB924QEVM evaluation board. The graphic and layout description are used to determine both proper routing and proper solder techniques when designing the Serializer board.

10.2 Layout Example