2.4GHz 45dB gain LNA PCB - Tell me all the things I did wrong - Page 1
Forum section: electronics / projects

author: TheUnnamedNewbie
author_rank: Super Contributor
timestamp: April 03, 2017, 07:18:02 am
content: So, as title says, I designed a 2.4GHz wifi-band LNA board. Should give me about 45dB gain in the band I'm interested in. Almost all passives are 0805, except those in contact with the RF signal path, those are mostly 0402. Powerlimiting PIN diodes on input and output. Amplifiers are MGA-637P8 from Avago (now broadcom). Entire board measures 60x25mm. Rogers 4350B substrate, 30mill thick, 17um copper. I've not been able to spam vias's everywhere or use CPW since the board will be produced inhouse, no soldermask or plated vias, everything done by hand.As you can see, it's pretty much 3 times the same amplifier layout in series, as each should get me about 15dB gain.D3, D4 and D2 are LED's that will light up depending on the powersupply (Vcc >5.5V, 5V rail on, and if the amplifier enable pin's are on or off).U1 is a 5V regulator, capable of 400mA. D1 is a diode to prevent damage when we manually apply 5V to the 5V rail from an external supply.A lot of manual tapers and curves added to just make sure we don't have any issues and such. Added cutouts to the pours to ensure soldering is easy (remember, no soldermask). Big hole under the 3 amplifiers is to be able to feed solder in through there. Don't know how it will work out, we will have to see.Testpoints are little rings I get from farnell. Don't remember their product number, but thats what they are, in case you were wondering.Things I'm currently unsure about: Should I make C6 and C16 0402 aswell? Did I make any other stupid mistakes? (I hope nothing to major since I spent a /lot/ of time on this board, I think a more than 20h easy)Schematic of the amplifier subsection:entire thing:Top:Top, seethrough (and mirrored, ups) (I use this a lot during designing since it's easier to see where stuff goes):Bottom:Bottom seethrough:

author: DutchGert
author_rank: Frequent Contributor
timestamp: April 03, 2017, 08:53:08 am
content: A schematic would help I think

author: TheUnnamedNewbie
author_rank: Super Contributor
timestamp: April 03, 2017, 08:59:22 am
content: Added schematics to original post. Note that the text in the schematics is not correct anymore, still busy updating them and building my BoM.

author: awallin
author_rank: Frequent Contributor
timestamp: April 03, 2017, 10:00:16 am
content: the amp can output +22 dBm but you are restricting to ~0 dBm with the diodes on the output?datasheet says 17.3dB gain per stage, so you are expecting less than -52 dBm of signal that gets amplified to ~0dBm?

author: dmills
author_rank: Super Contributor
timestamp: April 03, 2017, 10:43:22 am
content: My instinct says that an inter stage pad will help a lot with stability, 2dB or so will significantly improve the return loss seen by the following stage input and would not, I suspect, have any effect on noise temperature as it has 17 odd dB of gain preceding it.The decoupling caps around the amp chips would probably be better as 0402.If you are using end launch connectors you may want to mill a rebate into the ends of the boards so the connector flange faces are level with the edge of the board, it makes fitting the thing into a screening can less annoying.There are more doings on the back of the board then I would really be happy with, C9 & C11 in particular should probably 0402 with no vias in play.I am a little suspicious of the input and output trace geometry, they just look large for a 0.8mm board, but I have not actually checked.45dB is a huge amount of gain to have on one board at that sort of frequency, and it may be worthwhile doing some interstage bandpass filtering on board to minimise the overload potential, good RF design being about filtering everything you don't need out as early as possible after all.73 Dan.

author: TheUnnamedNewbie
author_rank: Super Contributor
timestamp: April 03, 2017, 10:49:36 am
content: The goal of this board is to drive a powerdetector to measure signal power in a certain frequency band (at first the entire wifi band, then start looking at specific channels if we have enough time for it). We want to measure right up from the thermal noise floor, which is about -100dBm given our bandwidth. The powerdetector (analog devices ADL5902, board has already been built and characterised) has a minimum input of about -60 dBm, measured in our mmwave lab at uni. Hence, to have some margin for the filter loss and such, we need about 40-45 dB gain, which is how I came up with the number. (the amplifier has about 15 dB gain in our frequency band, the quoted 17.3dB is at 1.7GHz)The maximum usefull input level of our detector in our band is about 5 dBm. To prevent the amplifiers ever giving out more power than that, I used limiting on the output to clap it to, as you said, 0dBm, since our detector isn't very linear above that anyways.

author: TheUnnamedNewbie
author_rank: Super Contributor
timestamp: April 03, 2017, 11:07:52 am
content: Quick extra note: This is going to be a board that will be manufactured once, maybe twice. Everything is done and verified by hand.Quote from: dmills on April 03, 2017, 10:43:22 amThat could be a usefull thing. I'll look into it. I was thinking that since the S11 and S21 of the amplifiers were so good, I needen't worry about reflections from the preceding stage giving me issues?Quote from: dmills on April 03, 2017, 10:43:22 amQuote from: dmills on April 03, 2017, 10:43:22 amI want to avoid 0402 as much as possible since we have to manually solder this thing without any plated vias, soldermask, silkscreen. I realise that it's better to use small components, but it's already a pain to get this type of layout populated (already, when my TA's looked at this board they said "you are going to manually solderthat?").Regarding the vias - I was thinking that since I'm in series with an inductor anyways, the added inductance of a trace would not be a big issue. Is this not the case? What should I worry about? It radiating, stray capacitance/inductance?Quote from: dmills on April 03, 2017, 10:43:22 amI'm going to write that down! I am affraid that our milling machine is broken tho, so I'll have to go talk to the guys manufacturing the pcb about it.Quote from: dmills on April 03, 2017, 10:43:22 amThey are 1.52mm traces. This has been verified by ADS and small testboards to verify the Er as function of frequency of the substrate.Quote from: dmills on April 03, 2017, 10:43:22 amI'm worried this will significantly increase the complexity of the design. I have little experience with this to begin with and am worried every component/building block I add is another one I can break/mess up/fail to understand.The system gets proceded by a bandpassfilter (different board - everything is being manufacturerd on separate boards for now for ease of testing). I think it will probably be followed by a gentle bandpass as well to avoid any spurious tones messing up our readings (the powerdetector can measure up to 9GHz, so...)Thanks already for the feedback!

author: awallin
author_rank: Frequent Contributor
timestamp: April 03, 2017, 11:27:41 am
content: although it's always fun to build stuff, have you looked at connectorized amplifiers from mini-circuits?Something like ZX60-P105LN+ sells for 77euros/piece and delivery is usually 1-2 weeks..

author: TheUnnamedNewbie
author_rank: Super Contributor
timestamp: April 03, 2017, 11:32:58 am
content: Quote from: awallin on April 03, 2017, 11:27:41 amThe point of this project is to build stuff ourselves!If my PCB fails, we can look at buying prebuilt amplifiers, but this is a design project at uni so I have to actually design stuff.

author: dmills
author_rank: Super Contributor
timestamp: April 03, 2017, 12:10:40 pm
content: The interstage pads are about having some sane return loss in places where the match is NOT good.S11 @ 2.5GHz is ~-11dB but at 100MHz it is -0.3dB with S21 at over 30dB, If the thing is going to honk, I would expect it to be down near DC, or up at 5Ghz or so. Incidentally 90dB of gain in the FM broadcast band might give you fits all on its own.Minicircuits probably have some sort of smt mountable filter that you could slap in between the first and second stage (and maybe also at the output) to limit the bandwidth, the XBF-282+ may be of interest (Integrated diplexer filter).You will in any case want to limit the bandwidth seen by the power detector to limit the total noise power.Incidentally those inductors need to behave at the highest frequency at which you have significant gain as well as at the frequency you care about, I might have been tempted to split R1 so that part of it was in series with the DC injection inductor to kill the Q, but that is just me.Regards, Dan.

author: soerenbnoergaard
author_rank: Contributor
timestamp: April 04, 2017, 09:22:39 pm
content: I agree with Dan. You have to make sure that your inductors behave as inductors at signal frequencies. If you go above self resonance you risk feeding a whole lot of power out to the supply and control lines. Depending on the isolation in your U2, you risk feeding a lot of gain from the output back to the input.In any case, make sure some of your decoupling caps on the supply and control lines are capable of killing the RF frequencies (20-30 pF, maybe).And making room for a pi-section between the sections seems like a good idea. You can always add some 0 ohm resistors or 10pF-ish caps in series in case you don't need any padding or filtering.Best,Søren

author: TheUnnamedNewbie
author_rank: Super Contributor
timestamp: April 05, 2017, 07:07:01 am
content: Thanks for the replies guys!Unfortunatly, I'm going to have to redesign most of my board since someone recently has bought up all the stock of the amplifier I need... (And I was so sure I checked its availability twice before starting the design...) So now I get to start over.But now I have a lot of pointers to keep in mind during that design, thanks guys!

author: cdev
author_rank: Super Contributor
timestamp: April 06, 2017, 03:11:53 am
content: Don't wifi amps need some kind of switch for rx/tx?I've never been able to successfully pull off multiple (rx only) LNAs in series on the same board.Admitted I was just trying to do it myself, used FR4 and could have put more into it but I just decided to use two standaline LNAs (for something I was ted to try) That worked well + was easy. For some reason my LNAs have always preferred to be connected to some coax on both input and output.- probably the weird antennas I hook up to them.The power lines in particular wanted to be separated and well decoupled. Ive never gotten a setup like that to behave. It oscillated and created broadband RF noise. I never figured out what was happening.You could zig zag so the traces are at right angles?Also, for the power - They make SMD feed through caps (3 terminals) for power. Ive never used them- I would try that on each positive DC supply lead. You can also make small copper shields separating the stages with a little cutout to go over the chip. 2.4 GHz is high to get it to work right making your own boards. If you want need it to look pretty and work the first time thats a pretty tall order. You can make small shielded boxes with tin on your PCB.I use 1000pf feedthrough caps for the power lead. That should make even a broadband LNA happy. You could make sub boxes inside of a larger PCB box. The first input capacitor is the most important one for overall performance. Keep the line on the input short. I also think the traces look way too wide.You can use caps side by side or piggyback, even dc block caps.A big part of success with MMIC LNAs is getting the best grounding you can.