How I populated surface mounts parts on both sides of a board

I’m working on a Low Noise Amplifier (LNA) for 1090 MHz. The PCB has surface mount parts on both sides, so the challenge was how to get the solder paste mask on the board when one side is already populated.
Enclosed is a set of pictures of what I did. The plan is to use rubber feet to lift up the jig that holds the board and has the stencil taped to it. Then put down the same rubber feat on your table surface in a place where there are no parts on the populated side. You can then place the board with “2nd side to be populated” up and apply the stencil and paste as needed.
I Lucked out with the design because I wanted a switching supply on one side of the board, and the LNA on the other. So I had some blank space on the board. The next time I do a “parts on both sides of the board” I’ll place areas for rubber feet on purpose, most likely where there would be mounting holes.
Enclosed is the KiCad 3D view of both sides of the board, and the pictures that show the approach taken. Feedback is solicited, I’m curious how other solved this problem.
If there is interest, once I do a bit more testing I can make a thread on the LNA project itself with focus on the methods used to layout the board (particularly how to have a switching supply and LNA on the same PCB).
Don’t know if I can upload a .pdf, that might be the best way to do that post. Just write up the project and upload it?
The switching supply side of the board:

The LNA side of the board:

The first step is to put the rubber feet on the bottom of the jig you get from OSH stencils (small cat hair is optional):

Then you place rubber feet on your table top/static mat matching the areas on the already populated side of the PCB where there are no parts (I populated the switching supply first):

Now you can put the 2nd side of the board on those feet. The top of the jig and the top of the board are at the same height:

The “down low” view showing how the boards are at the same height:

You can now tape the stencil to the jig and apply the solder paste. I had to take some care because I only had feet under the lower part of the board, but that is where all the parts were. When I do this sort of project again, I’ll make sure I have clear spots (where the mounting holes are) at the 4 corners of the board so the board is more stable when squeegy-ing the solder paste down.

Comments welcome!
Bonus pix: my soldering and examination set-up:


It looks like you did a neat job of assembling your board; much better than my hand assembly. Did you use that “crescent wrench” in the photo for placing your smaller chips? :grin:

I have done some double sided by first doing the side with the fewest parts. Paste, pnp, baking.

Then I do the more complex side. Paste, pnp, when I bake, you just have to wait for the temp to come down to ensure you don’t shift any of the bottom layer parts.

The “crescent wrench” is most useful for placing the 0402 parts :wink: . But I also use it to change out the various tubes that go on the end of the hot air device. I’m not wild about the heating and hot air device I have, but, it fit my budget.
On a double sided .064" boards and 0603 parts, the hot air reflow works very well. It is quite the challenge to get the temperatures correct, particularly on the 4 layer OSH Park PCBs. The 0402 and small chips that only have pads on the bottom, with no metal exposed on the sides are a real challenge. It took 4 tries to get the LNA chip to solder correctly.
And as @iabarry points out, the “soak temperature” is more critical for double sided boards. No one likes a storm of surface mount parts raining down on the heater.
I’ve got a .064" design on the list of next boards, and it will be a win to do that with a majority of 0603 parts and chips that have either metal on the side or actual “legs”.
Finally, w/r/t/ hand assembly vs. reflow, the switching supply design/layout, which I have used before, came out looking very nice. The LNA design, with it’s 0402 parts where I had to tweak/unsolder/re-solder various parts to get the analog stuff right looks terrible. With the parts values known, I look forward to the next assembly to see if it will look cleaner. Pix enclosed to demonstrate what I’m talking about. Note in the final board pix, all the components of the LNA and the two SAW filters fit in the area of a dime (for my International friends, about 18 mm). I tried to solder down two 0201 parts, no luck. It’s humbling but good to know what your limits are.
Thank you for the feedback.

Back side with switching supply:

Front side with LNA and dime for size reference:

Close up of some of the switching supply. R4 is an 0402 I had to tweak, so it’s not as “clean” as the larger parts that went on clean and were not changed.

And now the ugly- the LNA which has a lot of hand soldering parts tweak. The ground planes (3 of them) made soldering even harder, had to use a 60W iron for some of the parts that had ground connections. You can tell which are the few parts that were not manually changed. Ugly, but the circuit works great, still testing and evaluating.
All this does shown what you can do at home on a modest budget though…
I should probably do a post on the ground plane strategy as it relates more closely to board layout stuff. When you’re working with RF the distinction between “What’s a KiCad/PCB focus” and “circuit design focus” blur. The PCB becomes part of the circuit design. R10 is on of the 0201 parts that I just could not get soldered on. :frowning_face:


I failed to say I use a $20 toaster oven for baking.

You appear to have SAW filters before and after the mmic.
What NF do you expect?

I have a few 0402 parts but I avoid using them unless there is no choice. They are likely to get lost in the drop of solder at the tip of the iron. 0201s? Forget about it. My default is 0603s on a minimum size 0805 footprint. I can understand that getting close connections to a fine pitch IC using 0805 footprints is like having 14 full grown cattle all eat out of one shoebox.

1 Like

The toaster oven approach is understandable, especially with the OSHpark 4 layer RF boards, it’s very difficult to get things soldered to a ground plane even with thermal reliefs. And then the “hand editing” of parts is rough too, but that is where the hot air device is handy.

The SAW filter before the LNA mmic chip (a Mini Circuits PMA2-162LN+) is because so many of the 1090 MHz ADSB systems get overwhelmed by local cell phone signals. The receiver dongles made by Flight Aware use single chip Software Defined Radios (SDRs) that are typically direct conversion recipes with A2D converters and digital samplers. It’s pretty easy to swamp the first mixer. Mixers without some degree of Band Pas Filtering (BPF) often struggle. The Flight Aware ADSB receiver dongle does have an LNA in it, and there is a SAW filter after the LNA which is part of why it works so well. They also have a discrete component BPF you can put before the dongle if the local interference is too great. It is a most elegant solution.
The SAW after the LNA was an experiment. Once you have the gain of the amplifier, tossing another 2.5 dB is not an issue. And if the LNA chip mixed any of the input signal with any residual power supply noise, it could produce some out of band signals that might confuse the SDR.

As for the noise figure, the LNA chip specification is .5 dB. Another learning experiment here is how well to SAW filters work in very low signal strength environments. While the loss is specified, there is no mention of noise when the input is at -120-ish dBm. Most of the time you see discrete component filters or cavity filters before the LNA, and then the SAW filter is downstream in the signal chain where there is more amplitude available. I don’t have a noise figure meter, they are a bit pricy. And I’m pretty good at coming up with excuse to by test equipment. :grinning_face_with_smiling_eyes:
I know a company that has one, and hope to give this a test someday. will advise.
There are good LNAs available in this frequency range, so in addition to just wanting an LNA this was a great time to learn about living in a 1 GHz world. It was a good time to experiment with how to put parts on both sides of a PCB, ground plane design for RF, tightly packed 0402s, switching power supply noise management in sensitive RF systems and the like.

@BobZ Indeed 0402 are a pain, but at these high frequencies they seem to be required. My standard go-to size used to be 0805, but I’ve gotten good enough that it is now 0603. For people starting out, I tell them 0805 with the “hand solder” footprint and then go from there. One lesson learned is that if you need a Hi Q inductor, you will want to investigate going to an 0603 part instead of a 0402. The larger size allows for a bigger wire so the Q goes up and the DC Resistance goes down.
This board had to be pretty much all 0402 for the LNA. The switcher is mostly 0603. I do like placing an 0402 in a .001uF to .1 uF range very close to the input and output side of switchers, and then put the larger caps next. This helps maintain a low Equivalent Series Resistance (ESR) across a broad frequency range. On this board, both the switcher and the LDO linear regulator have variations on a chain of caps from .001 to 100 uF values to really provide as close to an ideal cap as you can get. A the LNA chip there is a 9.1 pF close to the power input which is crazy until you realize it’s not.
It’s easier to remove parts than add them, and the cost to toss a few more caps on the board is in the noise. This is why “hobby boards” are more fun than “work boards”.

I realize we’ve moved into a bit of an electronics discussion, but, when your circuit board is in a high frequency or very log signal level world, the electronics and the layout become integrally entwined.

Gratuitous pix of the LNA frequency performance and schematics, just to show the crazy problem of getting clean power supplies. Also a pix of the conducted noised from the 5V switcher before it goes into the linear 4V regulator. All examples of when, in some designs, the PCB layout is part of the circuit.

Gain and filter characteristics. Note the small bump in the purple trace, which seems to indicate that the part is working with a noise floor less than the -120 dBm limit of the spectrum analyzer.

Here is the conducted noise at the output of the 5V boost-buck switching regulator as it goes into the 4V linear LDO regulator. Pretty standard performance, most of the noise is in the 1 MHz to 150 MHz range. The key concept here is how much the regulator (blue) is above the background (yellow). This is where the PCB becomes part of the circuit, as can be seen by some of the blue spikes.

LNA schematic (there have been changes). Left to Right analog signal chains are so easy to grasp, so hard to get right. Digital goes everywhere but noise is so much less of an issue. There have been some posts on what the style or “look and feel” of a schematic should be. I don’t claim this is perfect, but it probably not too bad of an example.

Switching supply schematic. Filtering the input power to keep the switcher noise from radiating out the power leads, multiple stages of filtering with a spread of capacitor values and sizes, and a two stages- the switcher on the bottom of the PCB, and the Low Noise LDO on the top with the LNA. Probing with the spectrum analyzer at each stage shows the importance of the surface mount ferrite beads and verifies the design. Note that the switchers, the LDO regulator and the LNA are all on their own 3 layer ground planes. The interconnection of power and ground between the ground planes is critical.

Bonus gratuitous pix: The 3D print design for the chassis which includes board spacers:

Apologies for the circuit design tilt here, but, when you are in low signal level or high frequencies, the PCB layout is now part of the circuit. Little side projects like this help you learn.


I have not used it myself, but apparently a good DIY method is to use a skillet with about 10mm of fine sand.

You first solder one side and let it cool.
Then you turn the PCB over and press it firmly into the sand.
The sand forms around all parts on the PCB, it distributes the heat evenly and it holds the parts on the bottom in place during the “liquid phase” of the solder.

A problem here may be that firstly parts are heated twice, and that they are at a high temperature for too long. Both these factors can influence reliability.

1 Like

Hi, Peter

That is an interesting design. The input voltage range is indeed wide. 1V (once it is running) to 15V. I would call that a sort of bootstrap operation. Is this for automotive applications?

For the skillet approach, I would think a bead thermocouple temperature device would be essential. My Fluke 51-2 meter has been useful a number of times. It may also make sense to get the Flir One for your phone to see if the heat is spreading evenly. I used the Fluke 51-2 to get the temperature of the surface of the LNA chip, the the Flir to see if there were any hot spots on the board.

When you get close in, there is some issue with aligning the visible outline with the thermal image, as you can see by the coin. But it did show the LNA section was dissipating the heat evenly (another win with 3 out of the 4 layers being ground planes) and that the switcher on the back was pretty much producing very little heat.
The thermal image would help to check that heat was being distributing evenly. You do have to keep in mind that the color coding “auto-ranges”, so the orange/yellow “hot” may not be hot at all.

Many chip specs how indicate how many “reflow cycles” they can tolerate. Another factor to consider when selecting parts. Your comment on reliability is spot on.

tnx for the idea!


Regarding the switcher, the 15V is a limit I put on the part (via the TVS) because I had 25 volt ceramic caps on the input. IIRC, the chip can go up to 25 volts or so. On a bigger 100W power supply I did, I had an 18V TVS but the input caps were 35 and 50V parts. Corroded battery terminals or flakey voltage regulators can reek havoc on a “12 Volt” car supply.
The low quiescent current and wide input voltage range is unusual for boost bucks, most of the parts out there are for single cell LiPo batteries, and as such they have a max voltage of 5.5V. The lowest current device is on back-order until early 2023. I have 60 on order… the chip shortage is spread evenly across all types of chips. The “If my input volts goes low once I’m running, I’ll use the output volts to power myself” is also a unique feature. But at even a 2.5 volt input, the 55 mA draw of the circuit would translate to about 130 mA of input current so you would be very close to hoping the PTC fuse. At even 2 volts in it would blow (and then reset when the load was removed, a nice feature especially if the LNA is up on the top of a pole).
Linear Tech parts (now part of Analog Devices) have always been more stable and forgiving than other manufactures. This part is very stable on a .064" double sided board. Most of the other boost-bucks out there these days have to have a 4 layer board with uninterrupted ground plane under them. However, the Linear Tech parts have always cost more. I’m guessing that they put some capacitors on chip to stabilize things and caps on a chip eat space. Currently, in Quality 10 they are now up to $9 each. Pricing on semis across the board is up 25 to 50 percent if you can get chips at all.
The wide input range of this part does make it ideal for automotive supplies. Most everything I working on is designed to be “vehicle powered”. The 15V TVS on the input is, however, on the edge of acceptable. A better mix would be 18V TVS and change the input caps to 10uF at 50V. In this design, with the 140 mA fuse, 15V is OK. The fuse introduces about 5 ohms of resistance, so with the 15V TVS (SMB package) you have a max voltage of 24 V at 24 amps- an unlikely current draw due to the PTC fuse resistance. Note also the the TVS and PTC fuse protect agains revers polarity.

Every nook and cranny of a design has wealth of nuances behind it. It is both part of the fun and part of the aggravation. I suspect this is why everyone has the list of go-to parts, just like everyone has their “style” when laying out a PCB.

RF is fun partly because of the challenge, but manual soldering 0402s is too much for me.
Good luck

It seems that you are being (at least nominally) conservative with your voltage ratings. Of course “load dump” Load dump - Wikipedia

can wreak havoc. I have not designed much for automotive application.

LT has a good reputation, although my own two personal experiences with their parts were not so favorable. On the other hand, a year ago I did an “innovative” power converter design…(doing some things not on the datasheet) with a TI LM5155 which IC I had never used before. This was a double risk. But it all worked well…

@LM21 You can see with the picture the difference between a reflow that was never touched on an 0603 and the LNA with it’s 0402 and I was playing with the values. If I had gone with the KiCad “0402 Hand Solder” I probably would have been better off. The hand solder option might be the best bet for when a design would benefit from 0402s. I know I moved from 0805 to the 0603 on a board that had the 0603 Hand Solder, and now that I’m “used to it”, I just use the normal 0603.
The footprint on the LNA chip was also very challenging. I wish the semiconductor companies would make larger package versions of a lot of their chips, seems like they are forgetting both hobby people and making prototypes for real products. This is sad and perhaps foolish since most engineers started out as hobbyist.

@BobZ I really like the WSON package and any other package with wettable flanks. If you extend the pads in the footprint about 3 mils, it become very forgiving when there is uneven solder paste (which you always get when using the OSH stencils and “squeegeeing” by hand). It also makes both visual inspection and testing for shorts between pins easy to do.
I see that the LM5155 part is out of stock at Mouser, with the next shipments coming in March 20, 2023. It has a 77 week lead time. Another “jellybean” power supply chip that is more at the heart of the supply problems than the big processor chips.
Every chip maker has clunkers. I’ve been lucky with Linear Tech and have used about 4 of their parts in various designs.
Regarding load dump, TVS values and input caps are part of the game in automotive. The challenge is finding a way to control the resistance of the wiring to the battery. Here I used the PTC fuse, on the 100 watt supply it was a wound ferrite for EMI with 16 gauge wire, a common mode choke with 16 gauge wire, and a lot of input capacitance. And then there is the 2oz copper of the PCB. It’s odd to think of the copper in the PCB as a part of the circuit diagram like that, but even at low frequencies often the PCB layout is a “component” in the design.
And finally, with ceramic caps it’s “nice” to have the cap voltage rating be at least twice the working voltage due to the effect that the capacitance goes down with DC bias voltage. The cap is typically tested at 0 volts with a sine wave.

At any rate, relevancy to PCB work: If you can get a surface mount package with wettable flanks, use it and make your own footprint. Check your lead times on parts, a perfect board that has to wait for a year to get parts is no longer perfect. Consider the “hand solder” footprints if various two terminal devices get smaller than you would like.

The loss in the saw prior to the Lna adds to the NF. Which makes Sys nf about 3db.

Which is why you need to do special things for input stages.

1 Like

Wow. I don’t think it takes that long to get from wafer start to finished devices. Time to go a wafer a while. :slight_smile: Gives me some guilt about designing in that chip but these days there is not a lot of competent multi sourced power conversion ICs. I had read that power ICs are among the leaders in the “chip shortage.”

Yes the voltage coefficient is really something; varies a lot with the capacitor. In recent years I think the MLCC layer uniformity has improved so voltage rating has improved. You can get a nominal 4u7 (or maybe a 10u0) 25V X5R capacitor in 0805 that is rated at 25V, but regardless of that nominal rating you really only get 1 or 2 uF at 25 VDC.

I just came down from my lab where my new board had quit running. I have a comparator oscillator which originally had a 22 nF X7R 0603 timing capacitor. I did not need any great accuracy or stability but the frequency was running about 5x high for reasons I have not yet figured out.

The next think I put in there (I think yesterday) was a 33 nF C0G 100V 1210 TDK capacitor. The oscillator frequency was about 67% of what I had expected with 22 nF. That supported my initial calculations.

Today I was doing some other testing on this board, and it quit running. It turned out that TDK 1210 sized 33 nF capacitor had turned into a 50 ohm resistor. I know that such larger sized ceramic chips can fail due to mechanical (or thermal mechanical) stress but I had not encountered such failures much on my bench. The odd thing is that it was working OK for a while and then quit. I have less than 5V on this capacitor and it is oscillating at about 1 KHz, so electrical stress is negligible. Mainly I wish I had put some through hole pads in this location for a radial metallized film capacitor; that would have been perfect for what I am doing.

I have encountered wettable flanks but it is not something that I have paid much attention to. When I designed the LM5155 onto a board, my client had the board assembled by an assembly house so I did not need to be involved in that aspect. This was a very small 12 layer board with a lot of other parts on it, including some 0201s. No…I did not do anything with those…

It’s kind of mindblowing if they really schedule shipments 11 years into the future…
(But on the other hand, with 77 weeks lead time it might be March 20, 2023, not 2033…)

I guess so. What is 10 years if we are on a great forum?

@hmk Some typos are funnier than others… tnx for catching that!

I’ve got another power supply chip that is in the same time range (over a year, not a decade :grin:)

Between typos, mild dyslexia and overly ambitious automatic spell correction communicating via keyboard is rough.