DS90LV047A

www.ti.com

SNLS044C – MAY 2000 – REVISED APRIL 2013

POWER DECOUPLING RECOMMENDATIONS

Bypass capacitors must be used on power pins. Use high frequency ceramic (surface mount is recommended)

0.1

μF and 0.001μF capacitors in parallel at the power supply pin with the smallest value capacitor closest to the

device supply pin. Additional scattered capacitors over the printed circuit board will improve decoupling. Multiple

vias should be used to connect the decoupling capacitors to the power planes. A 10

μF (35V) or greater solid

tantalum capacitor should be connected at the power entry point on the printed circuit board between the supply

and ground.

PC BOARD CONSIDERATIONS

Use at least 4 PCB layers (top to bottom); LVDS signals, ground, power, TTL signals.

Isolate TTL signals from LVDS signals, otherwise the TTL may couple onto the LVDS lines. It is best to put TTL

and LVDS signals on different layers which are isolated by a power/ground plane(s).

Keep drivers and receivers as close to the (LVDS port side) connectors as possible.

DIFFERENTIAL TRACES

Use controlled impedance traces which match the differential impedance of your transmission medium (ie. cable)

and termination resistor. Run the differential pair trace lines as close together as possible as soon as they leave

the IC (stubs should be < 10mm long). This will help eliminate reflections and ensure noise is coupled as

common-mode. In fact, we have seen that differential signals which are 1mm apart radiate far less noise than

traces 3mm apart since magnetic field cancellation is much better with the closer traces. In addition, noise

induced on the differential lines is much more likely to appear as common-mode which is rejected by the

receiver.

Match electrical lengths between traces to reduce skew. Skew between the signals of a pair means a phase

difference between signals which destroys the magnetic field cancellation benefits of differential signals and EMI

will result. (Note the velocity of propagation, v = c/Er where c (the speed of light) = 0.2997mm/ps or 0.0118

in/ps). Do not rely solely on the autoroute function for differential traces. Carefully review dimensions to match

differential impedance and provide isolation for the differential lines. Minimize the number or vias and other

discontinuities on the line.

Avoid 90° turns (these cause impedance discontinuities). Use arcs or 45° bevels.

Within a pair of traces, the distance between the two traces should be minimized to maintain common-mode

rejection of the receivers. On the printed circuit board, this distance should remain constant to avoid

discontinuities in differential impedance. Minor violations at connection points are allowable.

TERMINATION

Use a termination resistor which best matches the differential impedance or your transmission line. The resistor

should be between 90

Ω and 130Ω. Remember that the current mode outputs need the termination resistor to

generate the differential voltage. LVDS will not work without resistor termination. Typically, connecting a single

resistor across the pair at the receiver end will suffice.

Surface mount 1% to 2% resistors are best. PCB stubs, component lead, and the distance from the termination

to the receiver inputs should be minimized. The distance between the termination resistor and the receiver

should be < 10mm (12mm MAX).

PROBING LVDS TRANSMISSION LINES

Always use high impedance (> 100k

Ω), low capacitance (< 2 pF) scope probes with a wide bandwidth (1 GHz)

scope. Improper probing will give deceiving results.

CABLES AND CONNECTORS, GENERAL COMMENTS

When choosing cable and connectors for LVDS it is important to remember:

Use controlled impedance media. The cables and connectors you use should have a matched differential

impedance of about 100

Ω. They should not introduce major impedance discontinuities.

Copyright © 2000–2013, Texas Instruments Incorporated

Submit Documentation Feedback

7

Product Folder Links: DS90LV047A