How are transfer vias used?

Question

I watched a video on via basics by PhilsLab (Video: https://www.youtube.com/watch?v=WPT96w3eLAM), in which he discusses transfer vias. He presents the following picture to explain why you should place them:

He then provides an example in a PCB software:

Questions

1. I want to place transfer vias on signal traces when they switch layers (as mentioned in his video.) I'm uncertain if I understand the concept correctly. Let's say I have a 6-layer PCB. On the first layer, I place signal traces, and on layer 6, I also place signal traces. Now, if I need to transition from layer 1 to layer 6, I would position the GND via as close as possible to the switching via. Do I also need to have a GND layer on the first layer? In Picture 1, the GND via doesn't seem to be connected to the signal layers. It is only connected to the GND layer. Based on this, my understanding is that I should replicate this setup. What is your opinion? Below is an image illustrating how I implemented this in KiCad V7.

2. Should I apply this technique to a 6-layer board?

Answer 1

do I also need to have a GND layer on the first layer?

It depends on what kind of transmission line you are making.

For a microstrip line, the ground is on the layer "below" the signal trace. It's on layer 2 for a signal on layer 1 or on layer 5 for a signal on layer 6.

For stripline, ground is on layers above and below the signal. If the signal is on layer 4, then ground will be on layers 3 and 5.

For coplanar line, ground is on the same layer as the signal. Sometimes it's also on the layer below, forming coplanar line with conductor backing.

Whichever kinds of lines you use (and the two lines being connected might not be the same type), your "transfer via" needs to connect the ground layer(s) used by the first signal line to the ground layer(s) used by the second signal line.

Answer 2

#1 No, you don't need GND on layer 1. Return path will be following GND on layer 2, then gnd transfer via, then to GND plane on layer 5.

Depending how signal is looping, I think, side on which you place transfer via may matter. I would guess the best position for the GND via would be where the angle between top signal and jumper (red and blue) is smaller.</s. If not sure, place GND via on both sides of each signal via.

#2 Yes, especially for 6 layer board, because otherwise you would loose some benefit that you gained from having ground planes close to signals. The exception is, if you were jumping between 1&2, because the signal would be naturally getting closer to GND plane. So there is no point adding transfer via there, unless you also had copper pour on layer 1.

P.S. In practice, you don't need to be too concerned about transfer vias for the debugger traces.