1
\$\begingroup\$

I currently have a design that features a BLE SOC that interfaces to a PCB antenna. Both the SOC and antenna are placed on one side of the PCB. What I'd like to do is place another (different) BLE SOC on the other side of the PCB and either:

  1. Use the same antenna for both SOCs.
  2. Put another PCB antenna on the other side of the board, overlapping the first antenna.

I understand that if I try to use the same antenna for both SOCs, that matching it will be difficult because I'll have to use via to connect the tracks.

I think the preferred approach would be option 2, but I'm unsure whether having two overlapping antennas in the same board space (albeit on opposite sides of the board) will be a good idea from an RF perspective. Can anyone offer any advice?

I'm not intending to use them at the same time, I'm going to populate one of the SOCs, not both. I want to do this because I'm trying to migrate to the second SOC, but do not want to do it in one PCB spin.

\$\endgroup\$
5
  • \$\begingroup\$ Sounds like you need to find an antenna that relies on the ground plane to produce radiation away from the GP thus the two antennas will tend not to interact too much. That is your first task should you choose to take it. Asking for product recommendations is off topic BTW (just in case you were to ask me). \$\endgroup\$
    – Andy aka
    May 29, 2018 at 12:51
  • \$\begingroup\$ Using the same antenna for both is possible, there exist ICs that could allow this. However, doing so could require more work. Even without an actual switch it could be possible, but you need to take care of the transmitters not blowing up each others receiver. But I question why this is a problem in the first place - why do you want to use two BLE transcievers within the same system? Sounds a bit like an x-y problem to me. \$\endgroup\$
    – Joren Vaes
    May 29, 2018 at 12:59
  • \$\begingroup\$ I should have been more specific. I'm not intending to use them at the same time, I'm going to populate one of the SOCs, not both. I want to do this because I'm trying to migrate to the second SOC, but do not want to do it in one PCB spin. \$\endgroup\$
    – Ed King
    May 29, 2018 at 13:09
  • 3
    \$\begingroup\$ In that case, things change. It could be interesting to connect both to the same antenna using a simple resistor jumper, and then only populate the jumper you need. \$\endgroup\$
    – Joren Vaes
    May 29, 2018 at 13:19
  • 1
    \$\begingroup\$ ..I'm unsure whether having two overlapping antennas in the same board space (albeit on opposite sides of the board) will be a good idea from an RF perspective I am sure that that will not be a good idea unless the antennas have been designed that way. That will very likely not be the case. Even a non-operating antenna at such a small distance will influence the antenna you're using. I would want at least a couple of cm between antennas (for 2.5 GHz) before I call them "separate". \$\endgroup\$
    – Bimpelrekkie
    May 29, 2018 at 13:51

2 Answers 2

Reset to default
4
\$\begingroup\$

I'm not intending to use them at the same time, I'm going to populate one of the SOCs, not both. I want to do this because I'm trying to migrate to the second SOC, but do not want to do it in one PCB spin.

This is the key part to this question.

If this is the case, it is likely far better an idea to use one antenna and use something like a jumper resistor to switch the right SOC to the antenna. Alternatively, if this is a prototype board, you can connect both to the antenna, and expose the copper near the junction between the two (so no silkscreen/soldermask) and just use a knife or such to cut the trace to the one you don't want to connect.

\$\endgroup\$
3
  • \$\begingroup\$ I understand that this is a simple approach, but I'm concerned with matching. Won't adding a secondary path ruin the RF performance of both paths? \$\endgroup\$
    – Ed King
    May 31, 2018 at 15:53
  • \$\begingroup\$ That is why you should include a way to disconnect (with a trace you can cut right at the y-junction) or connect (with jumpers) the trace you are not using. \$\endgroup\$
    – Joren Vaes
    May 31, 2018 at 16:00
  • \$\begingroup\$ @EdKing I second that, jumpers are the standard solution to this problem \$\endgroup\$
    – Alex I
    Nov 9, 2019 at 5:29
0
\$\begingroup\$

Joren already gave you a perfect answer for what to do, so this is more of a comment...

"Put another PCB antenna on the other side of the board, overlapping the first antenna" - This may seem like an okay idea, but is actually a bad idea, for several reasons.

  1. A PCB trace antenna almost always requires nothing conductive near it - other than a ground plane in a specific place and of a specific size. Putting copper on the other side (whether it's an antenna or anything else) will detune it and/or cause lots of reflections, that's why most PCB antennas have a keepout that requires no copper on any layer, and also anywhere within typically a distance equal to their size (or preferably much further). They're detuned by dielectrics too, but less so.

  2. The two antennas will resonate together. If you prefer, since both are on the same band, the inactive one will receive a really strong signal from the active one - and then probably retransmit it. This will probably not work out the way you want (ie neither will work properly), but also probably will exceed the spec for whatever is connected to the inactive antenna (as most Bluetooth chips don't really expect a 0dBm-level signal coming into the RF port). The least bad thing that can happen is harmonic generation which is out of spec.

  3. Because of 2, the detuning is likely to be much worse from a nearby antenna than from (for example) simply any random nearby conductive object. I've ran Bluetooth antennas very close to a metal plate - it basically works, although the range is not good. I think running an antenna close to a second antenna could (for example) give you a bunch of directional gain (and correspondingly, directions with very low gain) due to intereference patterns. Whatever it does, you'd have to simulate or try it, but it can probably be summed up as "nothing good" :)

Now, since I do want to encourage you to get hands on experience with RF, what I would suggest is you take two PCBs you already have which have trace antennas, stack them the way you want, tie the grounds together (hopefully all along the edges or better) and then hook up a network analyzer to one of the antennas. The N1201SA is a decent inexpensive device of this type that shows you what's going on with your antenna (maybe not as accurately as a Keysight or Anritsu, but good-enough). You can cut a micro coax cable and solder the end to the feed point of the antenna and the shield to ground, the other end with SMA connector goes to the analyzer. Then, let us know what you see so that we can all learn :)

\$\endgroup\$

Your Answer

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

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