So I am starting to make my first RF circuit board. We will be using a PSoC4 BLE chip as the transceiver. I'm doing my best to follow their application notes, specifically this one.

I should add an RF test point so that I can tune the matching network once the assembly prototypes are built. However, I'm confused on where I should place it. Most of the references I've seen have said that you need two matching networks on either end of your 50-Ohm transmission line - one near the transceiver, and the other near the antenna. The test point should then go in between the two, on the 50 Ohm line.

However, in both the cypress BLE kit and the Cypress BLE USB Dongle, only a single matching network is used. So where does the test point go?

enter image description here

I followed the app note suggested practice for using their MIFA antenna design, and I will feed the antenna with a 50-Ohm microstrip. But I'm unsure about what happens on the other end of that that 50-Ohm line. Does it terminate at C14 (referencing the above schematic), or do I continue another 50-Ohm impedance line all the way to the RF pin on the transceiver? Do I place the matching network near the antenna, near the RF pin, or near the middle?

  • \$\begingroup\$ What are all your intended tests for a connector and what effects do you expect with/without those tests connected? S11 >15 dB over spectrum? Have you simulated and verified the antenna and HPF network alone already with/out case, with sensitivity to side of gnd plane yet? What connector OSX? \$\endgroup\$ Apr 14, 2021 at 20:10

4 Answers 4


First, I hope by RF test-point you're referring to a u.FL type connector.

Based on the PSoC 4 datasheet the module has a single ended 50Ohm matched output pin: "The RF transceiver contains an integrated balun, which provides a single-ended RF port pin to drive a 50-Ω antenna via a matching/filtering network". So you need to design a 50 Ohm line from the ANT pin (pin 12) all the way to the antenna and in between the components of the matching network. Also, the matching network should be closer to the antenna.

To place your testing connector, so that you can then measure the antenna impedance and tune the matching network accordingly, you can make a bridge with a series and shunt component, sharing one of the pads at the matching network side, between the module pin and the matching network, something like this:

enter image description here

NOTE: I used capacitor notation on this schematic. This bridge can either be accomplished with zero ohm resistors or a capacitor in the order of 100pF (for 2.4 GHz it's nearly a short circuit).

There's a similar assembly on Raspberry Pi Zero board, here's a picture for your reference: enter image description here

Another possibility, as has been discussed in the comments, is to use a switched coaxial connector like this: https://www.mouser.com/ProductDetail/Murata-Electronics/MM8030-2610RK0?qs=%2Fha2pyFadui6EZC%252BNwU5I446m3Z%2FkahugdGMg7kp0Gd%252Bvd0%252BzP64YA%3D%3D

But instead of placing it in parallel, these connectors are meant to be used in series. So place it in series in the 50 Ohm line, somewhere between the RF module output pin and the matching network, preferably, as close as possible to the module.

When a cable is attached to this connector the connection will be set between the external cable and one of the directions. So be very careful when soldering, because the footprint of the component is symmetrical, but there's a small mark on the connector marking which way it will connect when you attach an external cable. You want to make sure it will direct to the matching network + antenna direction, so that you can measure the impedance of this group and therefore tune the matching network accordingly.

Additional tip: After you tune your antenna, on further versions of your product, solder this component facing the module, so that you can use to test the output of the module for RF test functions. This can be useful if you're planning to go on with a commercial product and need to do certifications and such.

  • \$\begingroup\$ Yes, I mean an RF test point, something like this: mouser.com/ProductDetail/Murata-Electronics/… \$\endgroup\$
    – rothloup
    Apr 14, 2021 at 20:19
  • 1
    \$\begingroup\$ @rothloup that's a switched connector and you need a particular connector to use it. That connector would be placed differently from what I've described. For that connector you mention, it is placed in series between the module and the matching network. You need to be careful with the orientation when soldering, so that when you attach the cable to the board, the switch connects the cable to the antenna side and not to the module side. The connector is very small and the marking even smaller, so be very attentive. \$\endgroup\$ Apr 14, 2021 at 20:23
  • \$\begingroup\$ @rothloup to do something like they did on Raspberry and as I described, you should use a connector like this: mouser.com/ProductDetail/TE-Connectivity/2337019-1?qs=l4Gc20tDgJIuN7nS9rJkJw%3D%3D \$\endgroup\$ Apr 14, 2021 at 20:28
  • \$\begingroup\$ Ok, so what I'm hearing from you and from @Aaron's answer is that the pin and my traces are all already set at 50 Ohm, and the matching network is there to help tune the antenna. So I should place the matching network near the antenna, and my RF test point should be between the network and the antenna, whether its the switch-in kind I posted or the solder-in kind that you show. Correct? \$\endgroup\$
    – rothloup
    Apr 14, 2021 at 20:30
  • 1
    \$\begingroup\$ @rothloup sounds good. I'll update my answer to consider the scenario of using a switched coaxial connector as well. \$\endgroup\$ Apr 15, 2021 at 21:33

The only time you need a matching network is if you have two things that do not have the same impedance. So if the PA output isn't 50Ω then you need to match to that for your 50Ω PCB traces (transmission line) to the antenna. If your antenna is also not 50Ω, then you would need to match the transmission line to the antenna as well.

But as you indicate in your schematic, the antenna is 50Ω, so you should only need to match your PA to the transmission line (which should be 50Ω) and your are done!

As for the test connector, it's typically placed on the output of the matching network so you can verify that it is 50Ω.


If the matching network is made of 0402 components, at 2.4 GHz, they all will behave as lumped components.

By that I mean that the wavelength at 2.4 GHz in your PCB is much longer than the electrical length of the 0402 L and C components.

Having said that, it doesn't really matter where you put the L,C matching network.

Just don't put it too close to the BLE IC because PCB rework might be difficult.

How to design matching network of a system that has no connector for the antenna which is printed or embedded.

  1. Trial and error tuning

Nordic Semiconductor, 15 years ago, published an interesting application note on how to tune a matching network without a VNA.

You need a spectrum analyzer, an antenna, a solder iron, many L and C parts.

Source: https://infocenter.nordicsemi.com/pdf/nwp_013.pdf?cp=12_14

  1. Micro coax switch

Between the ANT_OUT of your BLE IC and the matching network put an RF micro coaxial switch connector like U.FL.

Desolder the BLE IC.

Connect a VNA to the PCB by a micro coaxial adapter connector.

Set the VNA to measure the impedance Z at f=2.4 GHz.

If Z is not close to 50 Ohm then change the value of a capacitors or inductors until you are satisfied.

Both the tuning methods have 2 things in common:

  1. You need to start with a certain topology of the matching network.

  2. The number of different L and C parts is a finished number.

If you want to find the best matching network topology, download the free trial version of Optenni Lab software.

LTE and 5G radio modem use active integrated circuits to match in real time the impedance of the antenna.

They are sophisticated integrated circuits.

As you might know, antennas impedance depend much on objects in close proximity: hand, head, walls, etc.


I would put it at the junction of L1 and C14.

  • \$\begingroup\$ Grace - Welcome :-) Here on Stack Exchange we prefer answers which explain things, and these tend to be longer rather than shorter. For example, compare the length of your answer, to the other answers given to this question. Can you edit your answer to improve it by adding more details, perhaps explaining your experience, calculations, reasons etc. for recommending that location for the test point? Thanks! \$\endgroup\$
    – SamGibson
    Apr 15, 2021 at 0:01

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.