characteristic-impedancetrace
Generally speaking, what time of signals should be designed to have a 50 Ω trace impedance ?
Some datasheets I've read have specifically mentioned 50 Ω but others have not.
Is it good practice to make every trace 50 Ω ? Should it be reserved for high frequency communication lines only ? UART ? USB ? SPI ? etc..?
Forget about clock or signal frequency. Think about edge rise time instead. A perfect square wave of, say, 320 Hz actually contains much higher frequency components:
You can see frequency components going right up to 2000 Hz (and they go beyond too). But if you slow the rise time of the square wave, then you actually remove these high frequency components.
As we add higher and higher frequency components, we can see the rise time of the wave getting shorter and shorter.
To decide what frequencies your signal contains, look at the rise time on an oscilloscope.
The rise time of a signal is usually considered to be the time taken to go from 10% to 90% of the amplitude. Once you have taken this measurement, the maximum frequency you should worry about is about:
freq = 0.5 / rise time
A 100MHz clock will be a big problem if the rise time is 10ps!
Unless you're doing high frequency stuff, where you need to start worrying about
transmission-lining your traces and properly controlling impedances, you should generally be fine with whatever size you prefer.
Thinner traces have higher resistance, thicker traces have more capacitance (particularly when over ground planes). The capacitive loading of thick traces over a closely spaced ground plane could potentially be an issue, though generally to encounter such problems, you are likely edging into the RF domain anyways.
Most modern logic devices have very high-impedance inputs, so higher trace resistance isn't that much of a problem. Realistically, there is a fairly broad range of trace-widths that would work fine in most low-speed logic applications. As such, I tend to just go with whatever seems to look best, but that's an entirely subjective measure. One advantage to slightly thicker traces is they're easier to cut and solder to, if you need to make board-hacks at some point, but anything can be modified if you have the time.
Best Answer
When to consider a digital signal fast enough to treat the interconnect (PCB trace) as a transmission line depends on two things:
As a rule-of-thumb(*) whenever the electrical length of the trace is longer than some fraction of the rise/fall time, you will see reflections unless properly terminated. You can use 1/3 to 1/5 for the "fraction".
As an example: 4"/100mm trace is about 700ps of electrical length (use your favorite 2D field solver to find the exact number). If you launch a signal out of a semi-modern FPGA with say 300ps rise-time down that trace, you are sure to get reflections unless termination is used. In this case 1/5 of the rise-time is 60ps and the max trace length without significant reflections is about 8-9mm.
Make sure that you understand that the frequency of the signal is irrelevant. Reflections can happen with a 1Hz signal or a 500MHz signal - it's the same mechanism.
Now you can easily avoid reflections on a longer trace by using series or parallel termination. That is what we mean when we say treat the trace as a transmission line.
And you can easily do this with any impedance. There is nothing magical about 50R. That said, almost all modern digital signals can be routed in 50R and it's a lot easier to deal with only one impedance on any layer in a multilayer PCB.
As to your question about best practice: On boards connecting two or more modern digital parts, all traces are analyzed for signal integrity and routing rules are created before layout. In 99% of the cases I have analyzed, 50R is selected as trace impedance - even for differential pairs like USB, PCIe etc.
(*) Be careful with rules-of-thumb. Technology changes fast enough that you have to understand this stuff or you risk using an outdated rule-of-thumb.
Just for the fun of it I ran some simple simulations for you in Mentor Hyperlynx. Here is the simple circuit:
Here is what happens if you do nothing (note the length of the trace/transmission line here is 2ns or roughly 1ft/30cm):
If we make the trace 60ps long (8-9mm) the reflections are almost gone:
Changing the impedance to some other value does not significantly change this picture. But if we want to use series or parallel termination, we need to know the trace impedance.
Lastly let me just show how it works with a series termination resistor. In this example, the series termination resistor is selected so the output impedance of the driver IC plus the series termination resistor matches the 50R of the trace:
The simulation comes out like this looking very nice even with this long trace: