I am working on 4-layer pcb design with PCIe connector and golden finger. I asked a question about power planes before:Necessary to put all power planes together for 4-layer pcb?

Now I have a follow-up question about the most significant signals TX and RX on the board.

Here is my pcb layout, pcb layout What I am now worried about is the place in the blue rectangular. These vias may cause problems on the high-speed signals. But I am not sure how serious that could be.

Thank you!

  • \$\begingroup\$ Are you making a standard PCIe riser card? If so, you shouldn't swap the TX and RX traces. TX on the top connector should go to TX on the edge connector. \$\endgroup\$ Commented Feb 28, 2020 at 20:51
  • 4
    \$\begingroup\$ Those vias force the signals to change reference plane, so you should probably have stitching vias (possibly and caps if the other ref plane is not also ground) to provide a return current path right beside each of the signal vias. \$\endgroup\$
    – Dan Mills
    Commented Feb 29, 2020 at 12:54
  • \$\begingroup\$ Thanks for the reply! The board is designed as a TX/RX swap board to connect two computers using PCIe. On this board, I have one PCIe X16 connector(could connect to computer 1) and one PCIe X16 golden finger(could connect to computer 2). \$\endgroup\$
    – Ruiying Wu
    Commented Feb 29, 2020 at 22:17

1 Answer 1


If you designed your PCB with a high-end tool like Mentor Graphics Xpedition, you can do a signal integrity analysis of the signals you're concerned about right within the tool set. This would be the best way IMO, as it would include all the stackup, trace, and via information.

You may be able to export your board stackup, layout, and routing information into a modeling/simulation tool like Hyperlynx. Done right, the model would include all the trace/via information to give you a high-fidelity simulation.

You could use a 3rd party simulation tool and build up your signal trace/via structure by hand. Key to getting this to work is to make sure the model you have for the via is accurate.

Finally, you could try to analyze your via as a stand-alone structure in a field solver like HFSS or CST Microwave. This would give you the s-parameters for the via, which you could heuristically look at and make an assessment as to whether or not the via(s) are going to cause you any headache. You also also chain together the s-parameter model of the via along with the trace in a tool like ADS and look at the results. Again, the key here is to make sure the model of the via accurately represents what you're going to have on your PCB.

EDIT1 - Added one more idea

This falls into the "rule-of-thumb" category. You start off with the rise/fall time of your PCIe TX and RX signals. You then turn that time into a distance - the spacial extent of the edge. The formula for doing this is about 6 inches/ns (the prop time of the signal in FR4 board material) × rise time [ns]. So a signal with a rise/fall time of 1 ns has a spacial extent of ~6 inches.

The next step is to compare the spacial extent of your signal's rise/fall time to the length of the via (or any other impedance discontinuity). If the via/discontinuity length is 0.1 inches, then its affects on your 1 ns rise/fall time signal is negligible. If you keep the via length the same (0.1 in), and decrease your rise/fall time to 100 ps, then the length of the via is 16.7% of your rise/fall time, and starts to impact your signal integrity.

Note that using this rule-of-thumb alone does not tell you how bad (or good) your SI is. But it can be used to assess whether to have to go to the more sophisticated/costly/time-consuming methods I mentioned earlier.


Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.