Altium Impedance matching for PCB Antenna

Thread Starter

Bernardo D. Campanher

Joined Sep 8, 2023

I'm designing a new product with 2 layers, 1mm PCB, FR4, 1oz copper and a TX 433MHz PCB Antenna, we already use a very common model from the internet in our products (Application Note 52 - MICREL) and works fine, but learning more about RF i founded some things:

1: For 433MHz you should use the 1/4 wave length rule witch gives 17,3cm length antenna, the antenna from N52 have 18,6cm counting all vias with a 1.6mm board.

2: Altium have a field solver so putting the data it will give you the width trace for impedance matching. The antenna model uses a trace width of 1mm but altium gives a width of 1.6mm (50 ohms 1% precision) on "single type" and 0.411mm for "single coplanar type" on the balun part.

Images: 1: My layout with 0.411mm trace Balun part with stiching vias
2: My Layer Stack Manager with the inputs

My 3 questions are:

I should correct the length of model antenna to match the 17,3cm for boards with 1mm and 1.6mm to improve performance?

I founded wierd that the model uses 1mm width for the antenna instead of 1.6mm which altium calculates for type single to reach the 50ohms, is this antenna model right?

I inserted the pcb values (you can se all on the stack layer manager image) on 2 websites and they give a width of 0.55 and 0.7 mm instead of 0.411? which one i should trust?

The 2 websites:

Images: 3: One site calculates 0.55mm
4: Other site calculates 0.7mm



Joined Jan 12, 2022
Random thoughts...

Did you use the velocity of propagation in air or in FR4 for calculation of 1/4 wavelength?

Try removing the solder mask layers from the Altium stackup (Dk = 4) to see how it will compare to web calculators.
The Micrel design is a coiled up half wave that is end fed. The ApNote states the resonance is 650MHz. For 433MHz the matching circuit has to bring the resonance down with capacitive loading. A straight quarter wave would be more efficient (it mentions this in the ApNote) but a quarter wave antenna needs a groundplane to work with that extends a quarter wave length in the opposite direction or perpendicular to the antenna track. While you can use the groundplane that extends under your circuitry as the antenna groundplane I have found that this can cause problems feeding Tx output power back into the Tx oscillator causing modulation distortion.
The online impedance calculators shown assume a solid groundplane under the track you want the transmission line impedance for. For the antenna there is no groundplane underneath so these calculators do not apply.


Joined Jan 19, 2021
Something else to consider in addition to the removal of soldermask, which I would only do if you use an ENIG finish or Silver plate for protection. As for the FR4 materials and the Dk value, if you specify on your FAB drawing that you need a specific impedance for that trace(s) and you are close to your values with your calculations, the FAB shop can and will adjust widths and or Dk thicknesses as needed to get you what you need. You should run your numbers by your FAB shop if you have one selected, and let them give you feed back on your values, they have the tools to do that and a good shop is going to have an applications person that will know and give you info to make it work. (It may be specific to them, but if you get it close, it should work for most shops.) Just some comments, your mileage may vary. ;-) Good luck.