Electronic – USB-C Connector: How to route signals

If you have a power plane on the third layer, this becomes the reference plane for the bottom layer. This isn't a large problem: you just need to place a stitching capacitor near each trace where it transitions from top to bottom. These capacitors will only be connected to vias; one to the Vcc plane and one to the ground plane. (This is shown in the doc you referenced.)

This allows you to keep your differential trace geometries identical on both the top and bottom layers.

I asked a related question here. There is good information in the answers.

The larger problem can be the impedance mismatch presented by the vias in the differential traces. There are methods to design controlled-impedance vias. This is a useful article from EDN which describes one method. I suspect most people use a 3D field solver instead of doing it "by hand" :)

Your tracing options won't make things any better if the board has high dielectric loss. First you need to remove all the nonsense like shown below:

This serpentine doesn't do any good. Make the traces as straight as possible, no wiggles. 10ps delay due to length difference won't make any noticeable change in the signal. If anything, do the length compensation at the connector, so the trace would remain balanced along your board if your concern is about RF interference. In fact, USB HS emits mostly at 480 and 960 MHz, which is quite outside the audio range.

Second, use L2 as ground reference. Do your power distribution in L3 in splits. Your board's component density is not that high for not be able to do proper layer stackup and get proper power distribution from inner layers. Some parts of L2 can be used too if necessary, just make sure you have 4-5mm of contiguous plane beneath you HS differential traces.

Third, if you still see some loss of amplitude, use USB3320 Vendor Registers and boost TX strength in Reg. 0x31.