PCB design suggestions for a high gain, multi stage 2.4GHz LNA board

[TheUnnamedNewbie]

Hi all,

For a uni project, I need to design an amplifier board that provides at least 35 dB of gain (with the amplifiers I've currently chosen it's 45dB) in the 2.4GHz ISM band.

I've chosen the BGA612 from infineon as my amplifier, and am going to cascade three of them to get my required gain.

However, I'm worried that coupling of the final output will feed back into my first stage and cause oscillations.

What are some good design suggestions/rules/tricks to keep the coupling as low as possible? (Without just making the pcb a lot bigger... Idealy the entire thing would be sub 5 cm long)
I have to use microstrip lines since we are manufacturing inhouse and I can't via stitch for grounded CPW. Every via has to be done by hand (ie, take a bit of wire, stuff it in, solder on both sides, trimm to length).

(I'm going to simulate the entire pcb in Keysight ADS/Momentum, but if I already know what to use to get a good performance, it'll be less tweaking and fiddling around in the end)

[whollender]

What are some good design suggestions/rules/tricks to keep the coupling as low as possible? (Without just making the pcb a lot bigger... Idealy the entire thing would be sub 5 cm long)
I have to use microstrip lines since we are manufacturing inhouse and I can't via stitch for grounded CPW. Every via has to be done by hand (ie, take a bit of wire, stuff it in, solder on both sides, trimm to length).

First of all, making the PCB bigger is actually counter productive.  Longer microstrip lines will radiate better, and are likely to couple more than shorter ones.

Other than that, some suggestions:

• Keep all RF traces as short as possible
• Make sure that the power supply lines to each amp have good high-frequency decoupling.
• You have excess gain, use it by putting fixed attenuators between the amps.  I would put 2dB between each amp, and at the output.  Don't put one at the input to maintain noise figure.
• Arrange the circuit so that the output trace is rotated 90 degrees from the input trace

Because this is at 2.4GHz, you can probably just do the first couple (decoupling and short traces) and be ok.

[TheUnnamedNewbie]

Thanks for the reply. Is it perhaps usefull to do half of the amplification on the op layer and move the other half to the bottom stage? Or would the via's I introduce into the signal path in order to achieve that likely introduce more radiated signal power than just keeping everything at the top layer?

I'll look at placing in the attenuators. One of the reasons I'm no sure I want to do this is because while now, we are hitting the thermal noise floor in our bandwidth anyways, if it works well, we might start narrowing the bandwidth to introduce lower thermal noise floor, and we will then need the extra gain.

I'll attempt to keep the board as small as possible.

[awallin]

some of the DIY amplifier+pre-scaler GHz front-ends for frequency counters that many people have built may serve as design inspiration. here are two I found but there are many more:
https://www.eevblog.com/forum/testgear/replacement-for-the-pm9610-prescaler-for-philips-pm6654-high-precision-counter/
https://f6itu.wordpress.com/2011/08/26/upgrading-aades-dfd4-frequencymeter/

[whollender]

Thanks for the reply. Is it perhaps usefull to do half of the amplification on the op layer and move the other half to the bottom stage? Or would the via's I introduce into the signal path in order to achieve that likely introduce more radiated signal power than just keeping everything at the top layer?

I'll look at placing in the attenuators. One of the reasons I'm no sure I want to do this is because while now, we are hitting the thermal noise floor in our bandwidth anyways, if it works well, we might start narrowing the bandwidth to introduce lower thermal noise floor, and we will then need the extra gain.

I'll attempt to keep the board as small as possible.

A via may not radiate terribly at 2.4GHz, but if you're doing the vias manually, you'll have to make sure to trim the wire flush to the surface so that you don't have any stubs.  It's probably not worth it anyway.  You mentioned that you have ADS, so you might have a try modeling different ways of going from the top of the board to the bottom (single via, double via, etc).  However, if you're limited to a double layer board, you'll be better off leaving one side as an un-interrupted ground plane, which isn't possible if you go from microstrip on the top to microstrip on the bottom.

If you're only looking at 2.4GHz and you want to be able to get close to the noise floor, you'll need to make sure you have a very narrow band pass at the front end, especially if you're  dead set on using these wideband LNAs.  You'll also want to shield the board well to prevent strong signals (FM, AM, etc) from getting into the LNA chain and swamping the signal you're actually interested in.

If you really need low noise, you can also look into cooling the front end, depending on what you're looking at (this doesn't work so well unless you're doing radio astronomy type stuff).

[German_EE]

Please make sure that you use plenty of decoupling on the power lead of each amplifier. Use an RF choke and bias resistor in the supply lead but (ideally) split that resistor into two components and have a decoupling capacitor to ground between the two.

The vias? In the past I have drilled holes in the PCB then filled them with conductive paint. The paint is drawn into the hole by capillary action and then it bonds with the foil on either side of the PCB, no soldering and no clipping wires close to the groundplane.

If you are cascading devices then the bias-t on the input can be eliminated for two of the devices.