Electrical Engineering Stack Exchange is a question and answer site for electronics and electrical engineering professionals, students, and enthusiasts. Join them; it only takes a minute:

Sign up
Here's how it works:
  1. Anybody can ask a question
  2. Anybody can answer
  3. The best answers are voted up and rise to the top

I am designing a PCB with the transceiver SX1231 (868MHz) with a SMA connector for the antenna. I don't know much about antennas. I would like to know if there is some parameters I need to be careful to keep the circuit adapted (to reduce reflections of the signal's power).

In another PCB that a friend developed, I see a lot of Vias (a bunch of them, one after the other) around the pads of the SMA connector, what is the reason of this?

Do I need to consider the width of the traces that connect the capacitors and inductors between the transceiver and the SMA connector? How can I calculate this? Do I need to take in consideration the material of the PCB?

Is there something I need to take in consideration about the ground planes?

Thanks for your help.

share|improve this question
up vote 4 down vote accepted

You need to learn about fixed impedance traces. A good resource for calculating the trace width for impedance is Saturn PCB Toolkit

Most SMA connectors have pins for surrounding the signal with ground plane, or SMT versions have recommended via surrounds. The idea is to surround the signal in ground, just as the outer braid does in a coaxial cable.

FR4 PCB material should be fine with the frequencies you are talking about. Designs are working on FR4 with no issues quite a bit above 1 GHz.

The important thing about not generating reflected signals is reducing impedance mismatches as much as possible.

share|improve this answer
Thanks for your answer. As I have a capacitor in series between the transceiver and the connector (datasheet page 78), the trace must have the specific impedance just after the capacitor? Or before and after the capacitor? (I have the same question for the inductors in series) – koike Apr 19 '14 at 20:30
That looks to be an impedance matching network. You want to keep all of those traces as short as possible and keep the SMA connector as close to the chip as possible. This makes the impedance not matter, as they are a lumped circuit. – Joe Apr 20 '14 at 2:49
So it does not matter the trace width, the permittivity I use and the dielectric thickness? Nice. What do you mean with lumped circuit? – koike Apr 20 '14 at 12:14

You should consider making your track impedances match your antenna. Here is a useful online tool but there are a few others: -

enter image description here

The results show an impedance of 50 ohm with a track width of 2.92mm over a ground plane 1.5mm away. PCB material has a permittivity of 4. These are all values I've entered and you can do the same.

Keeping impedances matched reduces reflected power. Vias have an inductance that can be significant at UHF (and above) and so when connecting a top track to a ground plane, several vias are used to "parallel" the inductors and reduce the effect.

share|improve this answer
Thanks for your answer. But if a trace is longer than the other, doesn't it increase the impedance of the trace? – koike Apr 19 '14 at 20:36
Impedance of the trace is determined by the incremental capacitance and inductance of the trace. This is dependent on distance between the trace and ground plane and the width of the trace. If you are using two signals and different lengths, then that is a propagation delay mismatch issue, not and impedance issue. – Joe Apr 19 '14 at 20:59
@koike - consider 50 ohm coax - it doesn't measure 50 ohms and neither does it measure 50 ohms per metre. When a signal enters the coax, at that instant a current flows (based on the signal voltage and the "characteristic impedance" of the coax). What other amount of current could flow - the signal is nano seconds away from the load so the cable (or trace) tells it how much. – Andy aka Apr 19 '14 at 21:16

Another thing to consider, beside impedance, is thermal relief for through hole connectors. Make sure the ground vias have such relief for good solder.

share|improve this answer

Your Answer


By posting your answer, you agree to the privacy policy and terms of service.

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