Single-Board Universal Module

you are right, I'm wrong.
A second filter can be thrown in if needed. The "filter" in the data sheet is just the typical buck output circuit. Leave room on PCB and populate if needed. There are also special SMT LC filters that may work. I kept it simple.

If you follow the suggested TI layout to a "T" it should work as advertised, thermal vias "22uF" output, and all.

I guess you have the diode leakages under control.

Should additional filtering be needed, it looks like you could fit it on the layer one? A zero ohm jumper after the switcher can also be useful in troubleshooting, and can be used also for an inductor or a ferrite bead.
Nice work.

I stumbled across this while looking for servo controllers. They seem to have found a way around getting FCC certification for their DYI RF board.

I'm not sure how legal this is, or if it would apply to the universal module, but if someone were serious about making and selling universal modules, it would probably be worth their while to discuss this option with a lawyer.

b.t.w. They use also rf filter at the output;
www.pololu.com/picture/view/0J3333

I took a look at the switch layout, and the new one is not in the repo, so I cannot see everything well.
But from what I can see there are a couple of things I'd do differently.
The footprint for the TPS62172 looks different than the datasheet, which also include two vias in the center pad. This I got burned on, trying to eliminate on this size part. With vias in the center pad excess solder will suck down the part to the pad, which otherwise may be rocking and rolling on the center blob, not making contact with an edge.

The two larger holes for the USB connector can be vias, tied to ground for better thermal and electrical grounding, I think these are holes for the plastic bosses in the USB connector.

The footprint geometry in the datasheet looks different, and I would follow it exactly, paste mask and all. There is not too much wiggle room on 2x2mm parts.
( Making the pads a little longer helps if you have to hit the lead-less part with a soldering iron tip.)

The traces on the VIN and EN can be combined and made wider, like the app-note.

The grounds on the CIN and COUT and very close to each other, there may be a circulating current between them so I'd keep the as close as possible.

Here is rough sketch.

The extra trace length on the SW pin to inductor could increase inductance which is OK, but loop size, and DC resistance is more important, generally, but for this little guy I'd think its OK.

I did not update the PS1 lib's smd sizes, according to TI, just added two vias and a larger center pad.

USB holes I changed to (0.9mm) vias. Top side routing changed a little.

I'm ignorant of the mechanical constraints. Do you have a .step file of the case?

bitbucket.org/deviationtx

If you want a better isolation between the power sources, with "no" loss, smaller, and maybe same price, you could use two pmos FET's.Gates can take +-20V, drain 30V. www.digikey.com/product-detail/en/SI2369...-T1-GE3CT-ND/4327755
I could upload those files, but I want to fix that TI layout first.

You probably solved the Schottky diode issue.
If both supplies are ON, the the intrinsic diode takes over, cutting out like 0.55V. The file below can be used with LTspice.

Excellent news!

+10

Using two p-MOS-FETs rather than two schottky diodes would also eliminate the need for a solder-in "LDO bypass" component, as the loss of the FETs (~30mΩ) and the 100% duty cycle of the TPS62172 (with a 430mΩ @ 3V switch) would be low enough not create too much voltage dropn (~100mV) with a 3.3V input.
Of course with both power supplies active, the p-FET diode drop takes over.