It depends on how far the LVDS driver is from your FPGA and the *rise time* of the signal (note not the toggle rate)

If the trace is greater than ~1/10 of the electrical length (rise time / propagation delay) then you will probably need to look controlling impedance and termination with a trace of certain width above a ground plane (microstrip) or between planes (stripline)

If less than this (i.e. your LVDS driver is close enough to the FPGA) then you should be fine.

A typical propagation delay for microstrip (a trace above a ground plane) might be 150ps/in. So if your rise time is say, 1500ps then your electrical length is 1500/150 = 10in. So a trace longer than 1 inch will need consideration (some would say 1/6 of the electrical length or 1.6in, see the NI note)

Often just terminating at the source will do, as the reflections will only "bounce" once, and power consumption will be lower than with other techniques. You can do this with a series resistor equal to the difference between the output impedance of the driver and characteristic impedance of your trace. So if your driver has an output impedance of 20 ohms, them your series resistor will be 30 ohms (assuming a 50 ohm trace - note the impedance can change a bit depending on logic state)

IBIS models and simulation help, and SPICE can model a basic transmission line. You may want to play around with a simple setup based on the notes below in SPICE to get a feel for it.

There are many other ways to tackle this, and a lot more to it than outlined above - here are a few decent app notes on termination:

Transmission Line Terminations - UltraCAD

High Speed Layout Guidelines - TI

Proper Termination for High Speed Digital I/O - NI

FR4 propagation delay

I only have a vague idea of what characteristic impedance

Characteristic impedance is the ratio of voltage to current (thus, an impedance) for signals propagating along the trace, which is determined by the balance of capacitance and inductance along the trace.

It should be dependent on the length and the frequency, how come it isn't?

Characteristic impedance depends on the ratio of inductance to capacitance. Since both inductance and capacitance increase linearly when the trace length increases, their ratio doesn't depend on the trace length.

Also, within limits, these parameters also don't change much with frequency, so again the ratio doesn't depend on frequency and the characteristic impedance doesn't depend on frequency.

Intuitively I should calculate the characteristic impedance of each pad-to-pad trace and make sure it is always 50Ohm. Is that the case?

If the driving circuits are designed to drive 50 ohm loads, then generally yes. You also want to provide matched termination at at least one end of the trace, and possibly both, depending on the details of your circuit.

Generally you don't have to make a separate calculation for each connection. You just look at your board stack-up and find a trace width that achieves 50-ohm characteristic impedance, and make all of your traces that width. You might use microstrip, stripline, or coplanar waveguide geometry depending on the circumstances of your layout. You would do a separate calculation for each signal layer on your PCB, and maybe for the different types of geometry (microstrip and coplanar, single-ended and differential) if you need to use all those combinations.

If the trace length is less than about 1/10 of a wavelength at your operating frequency, then you can often get away with using an unmatched trace.

## Best Answer

The 50Ω standard is basically just convention. There are various stories about how 50Ω came to be chosen. The article Anindo linked is good. There is also The History of 50 Ω or There’s Nothing Magic About 50 Ohms. But the long and short of it is that it is a compromise between low attenuation and power handling.

But it became the standard impedance when designing for transmission line applications way back when. When an IC datasheet says you need to design your PCB traces with a controlled impedance, then you're designing to compensate for transmission line effects. If the impedance of the trace is matched to the output impedance of the IC or source, you reduce the possibility of reflections which would lead to standing waves on the trace and cause all sorts of headaches. Since the designers of the IC are designing with transmission line effects in mind, and since 50Ω is commonly used by convention, the 50Ω standard proliferates.

But 50Ω is by no means special. From this paper on controlled solutions by Advanced Layout Solutions: