High frequency signal passing through PCB via - Page 1
Forum section: electronics / rf-microwave

author: dzseki
author_rank: Frequent Contributor
timestamp: March 28, 2019, 09:33:34 pm
content: Here is something I was wondering for some time now without me knowing the good answer.From time to time I see in datasheets/application notes that high frequency (think of ~500MHz) signal is not meant to be sent through vias on PCB because of the high inductance of the via.Of course for such statement the via should be specified with a little bit more detail, but what I was thinking is actually why the via would have larger inductance than the same piece (length wise) PCB trace on the same layer, especially when the via is filled with solder? -As the thicker the conductor the less the inductance for the same length, right? What am I missing?

author: ejeffrey
author_rank: Super Contributor
timestamp: March 28, 2019, 10:29:39 pm
content: It is perfectly possible to send signals at 500 MHz or much higher through a via. However, you have to be careful.The via inductance is almost a red herring. You are basically correct that the via itself has not much more inductance than a trace of equivalent length. The real problem with vias is that generally the return current also has to change layers. If you have a single-ended signal on a 4-layer board and go from top to bottom, the return current has to move from the upper plane to the lower plane. If both of those planes are ground, simply add some ground vias as close as possible to the signal via. If one of them is a power plane you will need to add a bypass capacitor or few near the via. Even so, the return current will have to divert quite a bit to go through the via or bypass capacitor and add more inductance than the signal via itself.Solder plugging a via doesn't make a difference as skin effect confines the current to only the outer surface of the via.With differential signals the return current is flowing through the other signal conductor rather than the ground plane. This makes things somewhat clearer-- just keep the positive and negative signal vias close together. Becuase you can't place the vias as close together as you run normal traces, you may have a slight impedance mismatch but it shouldn't be too bad. You can deliberately add a bit of capacitance to smooth it out if you need to.

author: TheUnnamedNewbie
author_rank: Super Contributor
timestamp: March 29, 2019, 07:48:08 am
content: Quote from: ejeffrey on March 28, 2019, 10:29:39 pmAnother issue at higher frequencies is the stub vias can form. Say you have a signal on a 6 layer board going from layer 2 to layer 3. Now your via, unless you have fancy micro-vias or back-drilling, will still go from layer 1 to layer 6. In other words, you get a 1-layer thick stub at the top, and a 3-layer thick stub at the bottom, which can cause act as filters at higher frequencies. Sometimes this can be tuned out by increasing the track with in that area to act as a matching network, but it is not easy.There is also the fact that high speed currents don't like sharp corners. A 90 degree bend will appear as somewhat capacitive, which is why at these high speeds we use bends or we have mitered corners.

author: ejeffrey
author_rank: Super Contributor
timestamp: March 30, 2019, 03:47:56 pm
content: At 500 MHz I wouldn't worry much about the via stub. I just made a 4 layer board with modeate care using through vias and still measured 20 dB return loss at 5 GHz on a via test structure. That is a signal going from layer 1 to 2, and a 30 mil stub to layer 4. I can probably improve the via slightly but the connector is mostly the return loss problem.If your transmission line is thin you also have to worry about the annular ring size. With regular through vias you also have to consider that the via punches a hole in the ground plane.

author: dzseki
author_rank: Frequent Contributor
timestamp: March 30, 2019, 07:39:49 pm
content: Thank you guys for the great information!

author: tggzzz
author_rank: Super Contributor
timestamp: March 30, 2019, 08:39:22 pm
content: Google for "Bogotin's rules of thumb". Start at rule 0, and work up to rule 33.

author: Mechatrommer
author_rank: Super Contributor
timestamp: March 31, 2019, 02:19:54 am
content: Quote from: tggzzz on March 30, 2019, 08:39:22 pmdoesnt come up with anything much. only some writing from keysight and signal integrity problem from Bogatin Enterprise... no rule until #33. if you be more specific i believe that will be more helpful. cheers.

author: rfspezi
author_rank: Regular Contributor
timestamp: April 02, 2019, 06:36:35 pm
content: I need to connect a 5 GHz signal from an end-launch sma connector to an inner layer stripline.What minimum via diameter would you recommend?

author: KJDS
author_rank: Super Contributor
timestamp: April 02, 2019, 07:46:29 pm
content: At 5GHz, I'd want an EM simulation unless I didn't mind losing lots of the signal on the first iteration of the board.

author: ejeffrey
author_rank: Super Contributor
timestamp: April 02, 2019, 08:24:20 pm
content: It depends on your exact stackup and transmission line geometries. A via diameter of 1/2 to 3/4 of your stripline width is a reasonable starting point, but yeah: back it up with simulations if you need good results.