10

I'm working on an IoT board and it is all laid out (LTE, GPS, BLE, WIFI - 30mm x 30mm -- VERY TIGHT).

As a design concession, I have to use vias to route some of the RF signals. There's no other way to keep the board that small.

I've impedance matched and tuned several RF boards. I'm using the same PCB material, so I am confident the 50Ω traces will be correct. And I have a VNA to tune the matching network to the antenna.

However, what happens when the 50Ω traces hit a via?

Is there an known equation for impedance matching through vias?

Should I even worry about it if the traces are 50Ω?

I have a matching network from signal out on the IC to the antenna, so is it a moot point? Just use whatever via you want, and correct the impedance at the matching network?

Leroy105
  • 1,837
  • 3
  • 21
  • 34
  • 2
    It'll reflect for sure, I've got a feeling there's no way you can maintain the impedance with vias. You must accept some performance loss. How long are your traces? If they're just some millimeters/centimeters, you might get away with it... [Edit] don't expect that I know anything about the subject :| – PkP Oct 17 '17 at 15:37
  • The longest trace is around 15mm. – Leroy105 Oct 17 '17 at 15:38
  • Hmm... build it and see what happens :) Try at least to keep the different RF signals isolated from each other as much as you can. – PkP Oct 17 '17 at 15:40
  • Yeah, I have seen another design that also compromises and is using vias. I'm not certain if LTE module in question has an RSSI indicator (it probably does, so I could at least compare vs. a sample board from the manufacturer). BUT -- ideally there is a known answer... anyone? – Leroy105 Oct 17 '17 at 15:44
  • 1
    Saturn PCB Toolkit has a via impedance tab – Matt Young Oct 17 '17 at 15:57
  • 1
    Please see [this](https://electronics.stackexchange.com/q/142250/38335) related question. One of the answers has a cool link on calculating via impedance by hand :) – bitsmack Oct 17 '17 at 16:18
  • You said "RF signals" but not what frequency band. You might not care about via effects at 100 kHz or even 100 MHz, but you might care a lot at 10 GHz. – The Photon Oct 17 '17 at 17:07
  • 2
    @ThePhoton, Actually he did specify the frequency bands: LTE, GPS, BLE and WiFi. That's 1.8G, 1.2-1.5G, 2.4G and 2.4G. – PkP Oct 17 '17 at 18:31
  • @ThePhoton -- I know this is your wheelhouse. I guess the most affected band is LTE, which has three bands ~900MHz/1700MHz/2300MHz (don't quote me on those bands, I am going off what I thought I read). Even harder to say, right? I'm guessing the ideal via is frequency dependent. 10mm extra would make this problem go away. – Leroy105 Oct 17 '17 at 18:33
  • @Matt Young -- good call, I'll check that out. I do have a feeling the via sizing is going to be dependent on frequency, and LTE is multiple frequencies. – Leroy105 Oct 17 '17 at 18:35
  • @PkP, if he named Ethernet standards, I'd know the frequencies off the top of my head, but those names aren't as useful to me as just saying 1.5 to 2.5 GHz. – The Photon Oct 17 '17 at 18:51

1 Answers1

7

However, what happens when the 50Ω traces hit a via?

The via can act as a capacitive or inductive discontinuity in the transmission line. It will make at least a small reflection.

Below 1 GHz, this discontinuity is usually too small to worry about unless you're doing something like precision radar work. Above 5 GHz, you'd generally want to carefully design your via to maintain impedance matching as well as possible. 1-2 GHz is kind of a messy middle ground where you might get away with an unmatched via and you might not. So you probably at least ought to make a best effort at designing a matched via.

First, you want to minimize any via stub. If you can, route from the top to the bottom layer, not from layer 1 to layer 3, for example. If you can't, expect a capacitive discontinuity from the stub. It's possible to "back-drill" the via to eliminate most of the stub, but that's probably not justified at 2.5 GHz.

Second, if you aren't routing between layers that share a ground plane (for example layer 1 and layer 3 might both use layer 2 as their ground plane, but layer 1 and layer 8 don't), then make sure there is a nearby path for return currents to move between the ground planes of the two signal layers. One nearby ground via is okay. Two or three is even better. If one layer uses a power plane as its reference, then place a bypass capacitor for that power net near your via.

Third, you can use a tool like the Saturn PCB tool (google it) to design the via diameter and antipad diameter around it as it goes through power and ground planes, to give the via a characteristic impedance matching your line.

Is there an known equation for impedance matching through vias?

There are at least heuristic formulas. Tools like Polar or the Saturn PCB tool can be used to find the via's characteristic impedance, which depends mainly on the via diameter and the antipad diameter.

Should I even worry about it if the traces are 50Ω?

At 15 mm trace length and 2.5 GHz, you're over 1/10 wavelength in trace length. It's probably a good idea to make controlled impedance traces, but it will probably not be too critical to get everything exactly right.

The Photon
  • 126,425
  • 3
  • 159
  • 304
  • Thanks sir. I haven't actually built anything in the 2.5GHz range. I am re-laying out this board again (which is an agonizing 6 hour process), I see what you are saying with the layers order and vias. Unfortunately, I do have the signal going from bottom to top. Saturn PCB Tool -- thank heaven, I don't want to calculate that by hand based on a link I saw earlier. – Leroy105 Oct 17 '17 at 19:11
  • Top to bottom is good because there's no stub on the via. But slightly bad because you'll need to have return current paths also (assuming more than 2 layers total). If you have ground planes adjacent to both signal planes, that's really not a big deal. – The Photon Oct 17 '17 at 19:13
  • Yes, it's a 4 layer board (right now!). There is not an adjacent GND plane to the bottom layer. For the first turn, I should spin it as a 4 layer and see. I suspect this will take few turns of the board to get things nice and happy. – Leroy105 Oct 17 '17 at 19:21
  • Save your self the time and don't even try to go for a 4 layer board if the RF trace on the bottom doesn't have an adjacent ground plate below (or above, depends how you look at it). Maybe you should show the layout of the RF for a review here. – Mike Oct 17 '17 at 20:47
  • @Mike -- you've tried this before with a 4 layer board? – Leroy105 Oct 17 '17 at 21:52
  • @Mike, if there's not much clutter on "layer 3" (the one that isn't a signal or ground plane layer), it should work okay. Although the trace width for 50 ohms could be pretty large. Leroy, can you avoid having nearby traces on layer 3, or put a ground fill beneath the layer 4 trace on layer 3? – The Photon Oct 17 '17 at 21:57
  • The stackup is Layer 1 top layer, Layer 2 GND, Layer 3 Power, Layer 4 bottom (standard 4 layer stackup). Trace width for the 50 ohms on the 4 layer material is .304mm. Both the GND & Power layer have no signals, just vias cutting through them. Why are the traces on layer 3 a concern? I suppose I could put a ground fill on layer 3, and cut up the power plane underneath the trace in question. – Leroy105 Oct 17 '17 at 22:06
  • 2
    Tracks on layer 3, if they're parallel to the signal track on layer 4, could get some signal coupled from the signal track. Perpendicular tracks on layer 3 are not likely to cause a problem. If you have a power plane on layer 3, you can use that as the return path for your RF track, but you need to think carefully about how the return path connects to the source and load (and put bypassing near your vias as I discussed in my answer). – The Photon Oct 17 '17 at 22:09
  • I've been going through this for an hour. I wasn't familiar with the term reference plane, so I had go through that and current return paths. I think I have a loose understanding. Regarding the the power plane as the reference plane, you are saying to place a decoupling cap that goes to GND (through a via) and VCC (through a via). Place that right next to the via. Those vias, that the decoupling cap is using, provide a quick current return path to the top and bottom layers? Does it matter if that decoupling cap is on layer 1 or layer 4? I think no, because it is really the vias you want? – Leroy105 Oct 17 '17 at 23:32
  • I also had to look up backdrilling -- that's not cost feasible for the project. ;). I get what you are saying with the via stubs and reflections. – Leroy105 Oct 17 '17 at 23:33