GND Return Path Stitching  Via Design for High-Speed Signals in 10-Layer PCB - Page 1
Forum section: electronics / projects

author: electronx
author_rank: Regular Contributor
timestamp: June 03, 2025, 03:29:14 pm
content: Hi everyone,I'm working on a 10-layer PCB design with high-speed signals and need some advice on return path via placement.My setup:10-layer stackupUsing buried and blind vias for high-speed signalsSignal trace routing: Layer 1 → Layer 3 (trace routing)→ Layer 10Planning to add stitching return path viasQuestion:I know we definitely don't want a stub on the signal via (that's why I used blind and burried anyway) what about gnd return path vias?For the return path via, which approach is better for signal integrity:Parallel return via Gnd- Same length as signal via (L1→L3) and (L3→L10)Longer return via Gnd - Full stackup length TH (L1→L10)I understand that return current wants to follow the shortest path, so I'm leaning towards option 1, but I'd like to hear your thoughts on:What surprised me is that only a parallel gnd return path insertion to the signal caused an improvement in looseness (with an electromagnetic resolver)It contains a lot of vias, I wonder if there are any other effectsThanks in advance!

author: Niklas
author_rank: Frequent Contributor
timestamp: June 04, 2025, 08:21:10 pm
content: The signal on L1 will use L2 as the reference plane. When dropping down from L1 to L3, L2 will still be part of the reference for L3, in combination with what is on L4.Dropping down from L3 to L10, L9 will be the reference for L10. Given the blind vias L1-L3, I assume that the thickness of the dielectrics between L1-L2 and L2-L3 are thin based on typical aspect ratio of laser cut vias. Then having a drilled via from L1 to L10 would not be very much longer than a via from L2 to L9.Not sure it is worth to do a burried via. What is more important is the placement of the reference via(s) with respect to your signal via. Hint: they should be close.

author: ejeffrey
author_rank: Super Contributor
timestamp: June 04, 2025, 08:49:44 pm
content: A stub on the GND via won't have any impact. It's at ground potential, so it can't radiate. A thru-via will contact all intermediate layers and the current will only flow between the reference planes. It won't flow a longer distance just because your via extends past the reference plane.Also, I'm not sure what frequency you are operating at or what your SI requirements are but you should consider back drilling instead of blind vias. It doesn't reduce the stub to zero because there is drill tolerance, but it significantly reduces it. The small remaining stub is heavily screened by the ground planes because it is recessed. If you really want the best match you may still need blind vias but if your main consideration is crosstalk drilling can be just as good.. This will reduce your costs and manufacturing time significantly as they don't have to do multiple intermediate drill+plating steps.Also really make sure that you have confirmed the exact process with your PCB manufacturer. There are restrictions on where blind vias can end: generally they have to end on a core, not prepreg. I had a case where I had a prototype that was working fine except for a small discontinuity from the via stub. I asked them to add blind vias and they changed the stackup to something that was nominally equivalent but totally destroyed the performance.