Electronic – How differential pairs should be called out on fabrication print

First, in general, closely coupled differential pairs are somewhat above 50 ohms when each side of the pair is measured single ended (60 to 65 ohms is common).

A differential pair with each single ended signal at exactly half the differential impedance cannot (by definition) be coupled to each other, although many such scenarios exist.

That said, in a differential pair scenario, what matters is retaining the differential impedance; if the pair single ended signals move apart but retain the differential impedance, then there is no differential discontinuity.

If the differential impedance changes (regardless of the single ended impedance), there will be a discontinuity as given by \$\Gamma = \frac {Z_1 - Z_2} {Z_1 + Z_2} \$ where \$Z_1\$ and \$Z_2\$ are the differential impedances and \$\Gamma\$ is the reflection coefficient for voltage.

From the text, this appears to be a USB high speed interface.

The signal pair will have very little current, but you need to keep losses to a minimum.

The losses in high speed tracks are dominated by:

Skin Effect. This is because as signal transition rates become faster, the self-inductance of the conductor forms a high impedance in the centre of the conductor. A wider track reduces this loss (but it has diminishing returns above about 8 thou).

Dielectric absorption also causes losses. There is an excellent description of them here.

Another cause of losses is differential to common mode conversion, usually caused by a length mismatch between the pair.

The practical implementation of a controlled impedance pair depends whether you have a plane layer which is immediately below the signals; I will assume for now that you do and it is spaced 5 thou away from the signals (implies a 4 layer or higher PCB). The actual distance is determined by the various requirements of the PCB; a 5 thou core is commonly used (although many thicknesses exist).

I usually use 6 thou tracks for USB high speed (a decent trade-off for skin effect and PCB real estate); the gap between the pair can now be calculated by any number of tools.

For the geometry above, my calculations yield a trace separation of 4 thou using 1 ounce copper (commonly the finished thickness on outer layers).

If you do not have a plane layer, there are other techniques such as differential coplanar waveguide; just what technique I use is determined by the PCB geometries.

There is no one size fits all, but using a 5 thou to 6 thou track width as a starting point helps narrow things down.