I'm designing a board which contains an LTE module on it. I am a little confused about designing the trace between module and antenna.

As far as I know I need to match these:

  • Impedance of module's antenna output
  • Characteristic impedance of the transmission line
  • Impedance of antenna

Impedance of module and antenna are noted as 50 ohms in their documents. In that case I need to design a transmission line which has characteristic impedance of 50 ohms.

I am planning to use coplanar waveguide with bottom ground layer as transmission line. (2 layers board, 1.6mm board height) I tried a couple of online calculators and Appcad to calculate values for trace width and spacing to get 50 ohms impedance. I couldn't find any suitable values for my design because of pad widths of other components and restrictions of manufacturing process.

Is there any way to match this characteristic impedance with external components, like pi matching network? Or is it just related to trace width and spacing (also dielectric thickness copper thickness etc)

I tried to make an adaptable design. I added a pi network to match transmission line impedance (?). I added a high pass filter which is recommended by module manufacturer. I also added an extra uFL connector to connect VNA. Is it a good way to do like that?

enter image description here

  • 1
    \$\begingroup\$ What frequency band are you operating in? \$\endgroup\$
    – The Photon
    Aug 2, 2019 at 16:19
  • \$\begingroup\$ @ThePhoton It is an NB-IoT module. So frequency will vary depending on region or service provider. It seems 2 main frequency ranges exist, 700-900 and 1700-1900 MHz. \$\endgroup\$ Aug 2, 2019 at 19:46

1 Answer 1


It's ideal when the trace width ends up being the same width as your pad because the pad simply works as an extension of the transmission line. However, in most cases this is not possible, but don't panic because this is not the end of the world. When the pad is much wider than the 50Ω trace it's a good idea to have a void on the ground plane(s) immediately under the pad to reduce the parasitic capacitance represented by the pad and the GND underneath. The module and the antenna manufacturer (I'm assuming you're using a chip antenna) should provide guidance on what to do.

Having said that, simply use a 50Ω microstrip transmission line with the width you calculated based on the dielectric height and dielectric constant you have. I would use a clearance to GND on the top layer of at least two times the trace width. It's very critical that you place GND vias underneath the GND pads next to your module antenna feed pad. The same for the GND pads of your antenna (I'm assuming you're using a chip antenna).

I don't recommend adding a matching network for the purpose of compensating for the presence of a non-50Ω transmission line. The problem is that the matching will be narrowband and you need it to work properly over a wide frequency range. Having said that, it's always a good idea to have provision for antenna impedance matching (instead of transmission line impedance compensation). I would keep the pi network right next to the antenna you already have. I would keep the shunt components a little closer to the series component though. I can't tell what component size you're using - I would use 0201s (so you have a wider range of component values below the self-resonance frequency you can use).

  • \$\begingroup\$ Thanks for the answer. The antenna I'm planning to use is Taoglas Cyclone FXUB64.18.0150A. This is a flexible PCB antenna with a uFL termination. I'll keep in mind to fit the termination width with antenna pad. Is it okay if I use a trapezoid shape at the termination? So you're saying that if the widht of my trace is 0.6mm, I need to have a clearance of 1.2mm with the GND plane which is on left and right of the antenna trace right? Is it becoming a microstrip line in that way? So basically you said that I need to route as I calculate to get 50 ohms transmission line impedance? \$\endgroup\$ Aug 5, 2019 at 6:05
  • \$\begingroup\$ I see, you're going to have a connector at the end of the trace. In this case an extra advice I have is to keep the trace short since the loss (per unit of length) on the PCB trace is higher than the loss on the microcoax cable of the antenna. Looking at the return loss curve of the antenna you can see it's pretty narrowband at lower frequencies. You may be fine using the antenna as is, or you may have to add some matching to pull the resonance from 750MHz a little bit higher in frequency. A vector network analyzer would be useful for that. \$\endgroup\$
    – joribama
    Aug 5, 2019 at 20:00
  • \$\begingroup\$ At the termination on the connector side, I would void the GND underneath the connector pad; on the module side, I would not worry too much. Trapezoidal shape should be fine in both cases. Yes, keeping a clearance ~2w will make sure the impedance you get is close to what you calculated using a microstrip model, which is what I recommend using. Coplanar designs are not typical in cases like this. Yes, design it as 50Ω because both your module and the antenna are expecting to see that impedance. \$\endgroup\$
    – joribama
    Aug 5, 2019 at 20:06
  • \$\begingroup\$ thank you. I will keep your advices in my mind. \$\endgroup\$ Aug 6, 2019 at 12:21

Your Answer

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

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