Dear all,

I'm looking at incorporating a tiny bluetooth module from Murata into my design and I'm struggling with antenna matching circuit. The data sheet suggests there should be one, matching the 50 ohms. However, antenna is already integrated in the module. Shall I just put a 50 ohm resistor across antenna in and out pins? Why is it not integrated in the module then?


Thank you for your time,

Edmunds

 

As near as I can tell, the ANT-OUT and ANT-IN pins (13 and 14) provide an external loop for the antenna signal as it goes from the module to the internal antenna. It says it is for a pi-matching network. It's usually a series L and two C's to ground on either side (although when you do a full impedance-matching procedure there are sometimes other configurations of L's and C's within that Pi network). If you don't have a 2.4GHz Network Analyzer to measure impedances at high frequency, you can essentially short the two terminals together to make connection to the internal antenna.

For greatest flexibility in your circuit, however, you should lay out 0402 or 0201 resistor/capacitor type pads in the "Pi" network arrangement as close to the chip as possible, but with gentle curves in your traces to avoid points of changing impedance and radiation loss. Then, populate the series element with a zero-ohm resistors, and leave the parallel elements unpopulated. This is what they're trying to show you in the schematics. With these pads on your PCB, if you have poor range performance you can farm it out to someone who can do RF impedance matching with a Network Analyzer to determine the Pi-network component values for a better impedance match.

If you wanted to use your own PCB antenna, or perhaps something like a higher gain notch antenna on your PCB, or an external connector, you could run the ANT-OUT signal through a Pi-network for matching and run it to the antenna of your choice. (In this case you'd do nothing with the ANT-IN pin.)

 

FYI, RF impedance matching works like this: Using an RF Network Analyzer, without any connection between ANT-OUT and ANT-IN, you measure the impedance looking back into the circuit (ANT-OUT), and then you measure the impedance looking into the antenna (ANT-IN).

Note that this is not like measuring resistance with an ohmmeter. RF impedance is measured across a frequency band with generation and detection of signals in the Network Analyzer.

Once you've measured the impedances, there are online calculators to suggest Pi network combinations of L's and C's that will match the impedance of one side to the other. At the same time you can also check antenna resonance and try to optimize it with the matching network if it's really bad. If the antenna isn't at resonance, an impedance match isn't going to help it much.

But all this being said, you can prototype it with just the 0-ohm resistor connecting the ANT-IN to ANT-OUT and it should work passably well. If it's going to be a commercial product, I highly recommend doing a full resonance adjustment and impedance match.

 

Dear @InspectorGadget,

Thank you, great learning. I assume from the layout the antenna part is in the pad-less (upper half in the data sheet suggested pcb layout) area of the chip/module and thus have freed this from the GND plane and oriented it on the outer corner of the PCB. Could I route my "Pi network" on the underside of the PCB under the module? Or would that be likely to cause interference with the antenna above?

Thank you for your input,

Edmunds

 

You could put it under the module, but be aware that passing through vias will provide radiation loss points (because of the sharp right-angle turn from parallel to the surface to perpendicular and vice versa) and the vias themselves add inductance which will perturb the impedance matching. Better to take some real estate on the board and put them on the top.

Bring your trace out from the chip and make a straight path through the Pi network, and then come out the other side and make a gentle curve to loop back to the chip to the adjacent pad.