Does anyone have any experience using zero-ohm resistors in an RF signal path to select antennas? I've typically used RF switches for this purpose, but that's also when it was necessary to allow the antenna selection to be changed "in the field". But for cases where the antenna selection is a manufacture-time option, I'm considering simple zero-ohm resistors (i.e. populating one or the other to complete the particular signal path to the antenna).

Of course using zero-ohm resistors for this sort of thing in a digital circuit path is a no-brainer, but I'm specifically interested if there is anything I should watch out for since this is an RF path (two separate paths: 868-915MHz and 2.4GHz). Can I treat the zero-ohm resistor as essentially being part of the PCB trace, or will this cause problems?

PS - The two antenna path options are an on-board ceramic antenna and an off-board connector. The zero-ohm resistor would be a surface-mount component.

  • 2
    \$\begingroup\$ A zero ohm resistor will have a (slightly) different self-inductance than a track; whether that makes a difference in your design I do not know. \$\endgroup\$ – Peter Smith May 9 '17 at 15:08
  • 1
    \$\begingroup\$ A SMD 0 ohm resistor or capacitor should work fine. Just keep the "tee" part short where the signal paths split. 900 Mhz and 2.4 GHz are still fairly low frequency, and you aren't building a spectrum analyzer that needs 0.1 dB flatness over 20 GHz. If the tee junction is a problem you could use a wilkinson splitter and terminate the side you don't want. \$\endgroup\$ – Evan May 9 '17 at 15:56
  • \$\begingroup\$ @Evan--Interesting idea with the Wilkinson splitter, but as you say, I doubt it will be necessary. \$\endgroup\$ – eric May 10 '17 at 15:41

You rarely need DC continuity to an antenna, so I've always used a normal SMD 10pF to 100pF ceramic capacitor, depending on frequency. They're already used on the board, and tend to be cheaper than zero-ohm resistors, as we buy them by the bazillion rather than the handful.

  • 1
    \$\begingroup\$ That's a really good point! I'll go that route for now. \$\endgroup\$ – eric May 10 '17 at 15:43
  • \$\begingroup\$ What formula do you use to select the capacitor value? \$\endgroup\$ – eric May 13 '17 at 15:10
  • 1
    \$\begingroup\$ Other things being equal, and assuming that we're on a 50 ohm track, whatever value gives 'a few ohms'. Any more would start to influence the signal level. Any less is unnecessary and might start to cause other problems, like conducting low frequency noise, or generating a suck-out through an SRF that's too low with cheap capacitors. Hence my range of 10 to 100pF for your range of 900M to 2.4GHz. 10p/2.4G is about 6ohms, 100p/900M is less than 2. Maybe 6 ohms is a bit high, you shouldn't go any higher without careful thought, anything down to 0.1 ohms should be OK. \$\endgroup\$ – Neil_UK May 13 '17 at 15:18
  • \$\begingroup\$ Thanks for the quick response. What I'm trying to learn is how you derive those values. Is there a standard formula you're using to calculate the resistance (i.e. based on the track resistance, the center frequency, the cap value, etc.)? \$\endgroup\$ – eric May 13 '17 at 15:27
  • \$\begingroup\$ magnitude of capacitor impedance (ohms) = 1/(2.pi.f.C) (Hz and pF). The value of 'a few ohms' is not derived, it's 'rule of thumb'. 50 ohm impedance (not resistance) track is the most common one to use routing about on the board as it's (a) a convenient value to implement physically (microstrip width = 2 x dielectric thickness on FR4 and RO4350), and (b) it interfaces with 50 ohm connectors and test equipment, which makes debugging possible. Ask if anything else is unclear. \$\endgroup\$ – Neil_UK May 13 '17 at 15:40

Zero ohm resistors are commonly used in RF signal paths as a population option to select between an internal antenna and an external antenna. The key is to overlap one pad of the two resistors and make them at right angles to each other. For one example see Texas Instruments reference designs for their CC1310 Launchpad, CC1350 Launchpad, etc. Neil is correct too; sometimes we'll use 100pF caps instead. When in doubt check with the IC manufacturer; they know the RF part really well and can help.

  • \$\begingroup\$ Interesting (and makes sense). Do you happen to know if the 90-degree orientation is "required" or "better", vs say a 180-degree "T" orientation? \$\endgroup\$ – eric Jun 21 '17 at 16:49

Examine the geometry of your antenna track to ground W/gap ratio for controlled impedance. Thus a 1x2 LxW ratio is about half the inductance of a 2x1 ratio part. e.g. 603. 60x30 mil

Inductance is all about LxW ratio per unit length.

So a 1206 part has the same inductance as a 0402 but more capacitance and gap above ground plane depends on copper+solder thickness.

Normally a Pin diode is used for antenna switches.


Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

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