Cascaded LNAs Oscillating. Help please
I've got a a circuit with three cascaded LNAs (MGA-62563) and there is a lot of oscillation. I depopulated a LNA stage to simplify the problem to two LNAs but the oscillations still occur. The circuit is for GPS at 1.57542GHz, and I don't really care about wideband performance.
The oscillation is at 1.573GHz at ~10dBm and then a harmonic at 3.146GHz and so on up the spectrum. I have attached the schematic and an interactive PDF of the layout.
I have been playing around with different decoupling capacitor values and placing 1k resistors to ground at certain key points with limited success.
I made a really stupid mistake when sending the PCB out for manufacture by accidentally swapping the ground and power layers. So now there's the component and signal layer, then power, then ground and then another barely used signal layer. I realize this is not the way it should be but I don't have the experience to know if this is the root cause of my problem.
Any help and advice that people could give on the causes and possible solutions I would greatly appreciate.
Thanks in advance for any help you could provide.
Tom
You connected GNDs' of LNAs by thermal relief. LNA cannot see the GND well,and therefore those small inductances make the LNA unstable.
Instead, you should connect the GND pads by Flood-over and put some GND vias just underneath the LNA to complete the GND path..
Also, you have to connect the Drain Inductors ( L6,L7 and L8) to same side where the decopuling capacitors are connected.Otherwise RF currents will see a long path to reach to the GND and it will also make the LNA oscillate.If you cannot do this, place same amount of decoupling capacitors to the side where the inductor is connected to VDD.( I think the oscillation is mostly coming from this side)
Thanks for your response. That makes a lot sense, another one to add to the lessons learned pile and will make the change in the next revision.
Out of curiosity, how much of an effect do you think the mix up in layers makes? I don't plan on doing it again, it would just be good to know.
Thanks,
Tom
Since you don't intend to re-create the layout, you can make some minor modifications in according with my suggestions above.
For instance you can connect some decoupling capacitors to just end of the coil and GND,you can also solder the LNAs by scratching copper land . etc.
3 LNA chips in series is a lot. And there is NO bandpass filter part way down the chain to limit where a feedback oscillation can happen. And further, I see only the bare minimum of DC bias line filtering used--no series ferrite beads anywhere. Top that all off by screwing up your ground plane, and I am ROFLMAO. Get real.
Why do you need so much gain in cascade BEFORE you downconvert?
I implemented the changes you suggested today and it worked. The LNAs are now stable and giving me the expected gain. Thank you very much for your help.
I'll try adding the third LNA on Monday but I realise that might be a bit much to ask.
Thanks again.
Tom
I'm making a software defined GPS receiver. The minimum GPS signal level is -160dBm, with a 40dB active antenna gets me up to -120dBm. The MAX2112 downconverter IC I'm using has a minimum input power of -70dBm so I need 50dB to bridge the gap. Three MGA-62563 will give me 48dB of gain, a bit less than required but I'm sure the actual received power will be more than -160dBm in most real situations.
What would you suggest adding to the DC bias line filtering? In my research the only circuit I came across was the one I used, it would be great to know what I could do to improve it. This is my first foray into anything RF so I have a lot to learn.
Cheers,
Tom
Actually after writing my reply I realised the received signal power is -160dBW, -130dBm. So I don't actually need the three LNAs but doing more amplification with the discrete LNAs and less in the downconversion IC is preferable as the MAX2112 LNA has worse noise performance.
Tom
It's likely if you do throw your design into the friis equation you'll see that after the first 30dB of gain, you don't really get any improvement in overall noise performance. For example if your mixer NF is 10dB and your RF gain is 30dB, then your mixer adds 0.039dB to the total NF. If your RF gain is 40dB then that goes down to 0.004dB. Hardly an improvement considering the extra difficulty in stabilizing the amp with that much gain.
It's likely if you do throw your design into the friis equation you'll see that after the first 30dB of gain, you don't really get any improvement in overall noise performance. For example if your mixer NF is 10dB and your RF gain is 30dB, then your mixer adds 0.039dB to the total NF. If your RF gain is 40dB then that goes down to 0.004dB. Hardly an improvement considering the extra difficulty in stabilizing the amp with that much gain.
And yes switching the power planes would certainly make a big difference. In fact I'm surprised it works at all with a solid pour directly below the signal layer. Your microstrips are going to treat that as a return path (regardless of whether it's ground of a positive supply), and that spacing is probably just a few mils. Are you using controlled impedance for the PCB?
You make a good point, I will definitely consider dropping an amp or two.
I'm just using normal FR4, not ideal but I've heard that at this frequency the losses aren't too great. It's for a final year project so I'm limited by manufacturers and costs that the University are happy with.
Tom
FR4 isn't the issue I'm referring to. In fact when you put a copper pour on layer 2 (the inner layer under the top layer) the FR4 won't matter at all because the prepreg will be the dielectric for the resulting microstrip. So if you don't get controlled impedance, and resize your microstrips appropriately, your Z0 will be way off.
When implementing microstrips on 4 layer designs, I typically remove the pours on layer 2 around the microstrip and use a layer 3/4 pour as the return path. This will give much more predictable performance without having controlled impedance from the board fab.
I see what you mean now, no it wasn't a controlled impedance board. There's just under 8 mils of prepreg between layer 1 and 2 which I had plugged into a coplanar waveguide calculator to get track widths. That's an interesting technique for better performance that I will definitely look at using in the future.
Tom