@eepete : If you can afford the voltage headroom, you may consider a capacitance multiplier circuit before the linear regulator. Horowitz & Hill’s The Art of Electronics (the third edition and the subsequent supplement The X Chapters) discuss capacitance multipliers in detail. The following article in Analog Device’s Analog Dialogue shows a practical application of the capacitance multiplier. Zetex makes some nice transistors with low 1/f noise corner frequency. (Any low-frequency trash may corrupt the carrier through the miracle of modulation, so low-frequency stuff is very important in RF design.) Shielding the LNA may reduce radiated pickup.
Tnx for the idea, will investigate. As part of the ongoing investigation, I need to bring out the +4V after the linear regulator and see what it looks like. Solder a BNC to the 4V output, feed into spectrum analyzer. When I saw the schematic for the “capacitor multiple” in the link you provided, it range a bell. Haven’t see that in years…
In the first figure of the link you provided, you see what I have which is typical- a higher uH inductor for keeping the input voltage clean, and ferrite bead on the output to get rid of high frequency noise. I have 4 stages of this sort of filtering that match the “hopping across ground planes” in the layout.
All this is another example of “When the PCB layout becomes part of the circuit diagram”.
I don’t know how “good” of a modulator the Mini Circuits part is w/r/t/ Power Supply Rejection Ratio. Something else to try to measure…
If you look at the KiCad 3D view, you can see where there are traces exposed for a shield over the entire LNA section. I once worked 1 mile from an AM station (960 KHz) and any low level scope measurements were very difficult. Many good lessons are learned the hard way. I also still need to pull out my E and H field probes and poke around the power supply.
For anyone reading this that doesn’t know what the term “split ground plane” means, here are pix of the 4 layers of the PCB. You can see there are ground pours on all 4 layers. There is a switching supply ground plane on the top, the LNA ground plane on the bottom, and in upper part of the LNA ground plane is the 4V LDO regulator small ground plane. As the DC power for the LNA crosses each ground plane, it gets filtered again. There is a small connection between grounds on each ground plane, and the DC power trace always runs near this small connection. You can see this in the 3rd layer (purple). You can also see this on the top layer (red) coming out of the components in the upper part of the LNA area. This technique can also help with audio. There are, of course, many other ways of dealing with this for both RF and audio but this is a PCB forum not an electronics design forum. But this gives the reader some idea of “when the PCB becomes part of the circuit”.
I have had similar problems. I thought that may be connectors were too tight and the board flexed hen people attached cables into the connectors. I think and hope that (more) flexible capacitors would help.
@eepete: Welcome. One little gotcha with the capacitance multiplier is its output impedance: It is essentially the emitter output of a transistor. Therefore, to get low impedance, the collector-emitter current through the transistor should be high (at room temperature, the output resistance is 25/I, where the collector-emitter current I is in mA). One other comment: In your schematic, I see that the SAW filter is before the LNA in the signal chain. If its loss is 2.5dB, as stated, then your noise figure cannot be lower than 2.5dB. This is derived from the well-known formula of the noise figure of a cascade. Filters before the first LNA is always a balancing act because basically you cannot get back information (SNR) that was lost and the losses before the first LNA in the chain, as well as the LNA itself determine the noise figure of the cascade. (Similarly, the last couple of stages of the cascade determine the IP3.) So, one has to balance interference from strong adjacent channels, with all ensuing maladies, vs. deterioration of noise figure because usually a filter with sharper skirts requires more poles, so it is more lossy. You may want to investigate a distributed-element filter on a low-loss substrate (not FR4), although at these frequencies the dimensions of such a filter may not be desirable.
Thanks for the info on the capacitance multiplier. Sound like it’s not of value here, but always fun to learn about these sorts of things. I still have my 1970’s vintage Nation Semiconductor Linear Handbook and Linear Applications book. The impact of chip opp-amps is amazing.
Indeed, while the LNA chip is a noise figure of .5 dB, adding a filter before it increases the effective noise figure as you state. I have the ability to populate the SAW on the board (and plan to do so) because I have a transmitter in in the 902-928 MHz band close to the ADS_B antenna. I suspect I’ll build one LNA with pre-SAW, and one without and try the Flight Aware dark blue filter and see what they look like.
I am going to re-work the PCB now that I see that I’ve got the power supply noise gone from the 1090 MHz band. I’m going to put the switching supply on the top. The LNA section will have a shield on it. If this works OK, that will be an easier populate. But it was interesting to try a surface mount PCB with parts on both side.
I’ve taken to increasing the temperature on the solder system I have, making it harder to put the board on the bottom and re-flow on the top without making a shield for it. The higher temperature for the “soak” period is making it easier to hand re-flow the board, and produces better results for the larger area parts and ground plane pad on the bottom of chips.
So agree completely with all you say. It is indeed a balancing act. It will be interesting to see if there is any measurable difference between a SAW filter pre-LNA and the discrete Flight Aware filter before the LNA. A possible win of the discrete filter is it would be less sensitive to overload than the SAW. Someday soon I’ll get a 2nd RF generator (the one I have now is a 1994 HP 8647A that only goes to 1 GHZ). Then I can do better IP3 testing. FWIW, the PCB is the OSHPark 4-layer, which is good for RF stuff. I wonder if it would be even better if the 2nd layer was a bit further away so that a 50 ohm trace was the width of a 0402 pad. But then you might have more radiation due to the larger gap. I put a 100W boost-buck supply on that same 4-layer stack-up, but change the to and bottom layers to 2 oz copper, quietest switcher I’ve ever made. I cut a small PCB with SMA connectors on it to play with a discrete filter. The parasitics were nasty, passband was off by 70 MHz. So in the interest of time, I’ll just buy the BPF filter. The usual build-buy issues…
Electronics Design- finding the optimal set of trade-offs for a given problem. Thank you for your insightful reply !
Last time I priced it for low volume (100 units-ish) it was an extra 5 cents per part. This was about 15 years ago. They ran the bottom 1st, putting a dot of glue down and then the part. There was some cure time, then reflow. Of course, the parts had to be a subset of all parts and not have ground pads on them.
At the time, and I suspect this is still true today, there is a lot of variability based on what through hole parts you have, if they have to be done by hand, etc. The price is more “system parameters based” than “cost per part on the BOM.” With just about every stuff house able to run 0402, you see less of this today (baring wearables and other really, really small stuff). I tried it for better isolation between the power supply and the amplifier.
In summary, work with your assembly house as you do your PCB design, not as an after thought.
I turn them off… And I never make mistakes!