First project, can someone look it over?


D’oh, I thought of that right after posting.


Some links:


@Joan_Sparky so from what I gather, I should have a 10uF ceramic capacitornext to my power supply in this case, the power boost 1000c, and a .1uf tantalum capacitor next each vcc pin on any of my ICs? Does that sound right?

Everything suggests using SMT caps, but would there be any issue with using THT caps?

Something like this:


Some more thoughts:

1.- In your microcontroller do no put 1 bypass cap, but 2 instead: one 100nF and one 10nF in parallel.

2.- If you have decided to place a GND plane, make it in both cupper sides; and if you notice not connected isles, connect them with GND traces and repour the polygons.

3.- For GND plane you might use 20 mil clearance.

4.- Power traces should be as thick as possible, even twice from the calculator values.

5.- 90 degrees traces could lead to reflections and manufacturing problems … Think for a moment in a water pipe with 90 degrees corners: the water pressure will decrease with this kind of corners; same with electrons. That’s way 45 degrees corners are prefered.

5.- Traces from the crystal to the microcontroller should be as thick as possible. Also add a ground plane that surrounds the crystal, the caps and the crytal’s pins (check what your microcontroller’s manufacturer has to say about this in the user manual).


Why make both sides GND, why not one VCC and one GND? I know this also makes it a weak cap, helping with filtering.

Will using through hole Caps be ok.


So after digging around a bit, I realized the powerboost and the Bluefruit LE UART Friend, since they are separate PCBs, do not need bypass caps, because they have them built in. As a matter of fact, the bluefruit has a 10uf, then the 3.3v converter, then another 10uf, and finally a 1uf cap, while the powerboost has a 2.2uf and then a 100uf on its power output.

I assume that means my power supply (the powerboost) does not need that separate large cap.

Here are the schematics I used to figure this out:

nano or micro?


I think that you mean paste reflow, not solder wave


Over the years I was putting together a kind of checklist at:
It is not only relevant for EAGLE-designs but for general issues as well. I look forward to read your feedback.


updated to include filtering caps:


You generally use a Vcc plane when the current intensity in your circuit is expected to be very high. Besides that, a Vcc plane (aka power plane) is put in the internal layers (for 4 o more layers).

Also, you HAVE NO CONTROL on the capacitor that is created when ground a power planes are used together.

Ground plane helps with parasitics and EMI transmission/radiation.



‘n’ stands for nano, whilst ‘u’ stands for micro.



No, I meant wave-soldering (or wave solder). He is using PTH in one of the boards (the one with LEDs).

I hadn’t seen the other boards, and in fact, for those with SMD components one MIGHT use paste reflow as you’ve pointed it out, or hand-soldering as well.


I understand, but I what I mean is everything else says a 100nF and a 10uF, not 100nF and 10nF.

@fjrg76 @1.21Gigawatts @Joan_Sparky
Except for the gnd/vcc planes, does it look ok to you?


Signal tracks still look awfully thin for a THT board - what’s their width (mm or mil)?
VCC/GND are well taken care off.

PS: might be a little late to ask this, but how are you programming the AVR?
Atmel has defined an interface for that (ISP) which you might want to implement/use… if you get one of those AVRispMkII clones to do this etc. you can even debug the MCU in-situ.


@Joan_Sparky thinnest trace is 10mil. With a 10deg allowed thermal rise this can handle around 3/4 of an amp, well above the predicted draw on my lines (with the exception of power rails, I cannot think of anything drawing over 40 milliamps.

As for in circuit programming, I am not using ISP because of pin requirements of my project. I have instead opted to use the RX/TX pins. Since the chip already has the Arduino bootloader, I can reprogram the chip over that. In addition, I do not know how to use the in-situ debugging, so there is no point for me to set that up.


You only need one 10uF (or larger) cap on your board, preferably where power connects to the board. Every IC should have a 100n decoupling/bypass capacitor, usually on each of it’s power pins, keeping any traces as short as possible. Some ICs, such as microprocessors, might benefit from also having a 10n cap in parallel with the 100n. In your case this is probably not essential for 16MHz but wouldn’t hurt. It would be of more benefit for an IC such as a microprocessor that used a relatively low frequency external crystal (12 - 25 MHz) and multiplied that internally to a much higher frequency. Datasheets usually give some advice where decoupling caps are concerned, sometimes they even recommend a 10uF at the power pin of an IC in addition to the 100n and 10n.

Yes, THT is fine but again keep lead lengths as short as possible.

See! You can’t mention 90 degree corners on a PCB forum without someone regurgitating this nonsense. But of course, if you prefer, there is nothing wrong with mitered corners.

We all know how power hungry those crystals can be! :wink: Crystal oscillator circuits are high impedance so wider traces aren’t going to help there. The inductance of a 10 mil trace 0.5 inch long is 8nH, increasing the width of the trace to 20 mil gives an inductance of 7.69nH. Not exactly worth the effort. More importantly keep all other traces away from the oscillator area. As mentioned, some datasheets advise having a ground ring surrounding the oscillator circuit.

Having in circuit programming ability can be quite handy when you brick your board. Many processors also provide a JTAG interface for this purpose. You can always add the footprint for a connector to the PCB but not populate it until you need it. You’ll learn how to use it quickly enough once you need to. :slight_smile:

I can’t make out much on the schematics you posted.



I will look into using the ISP, but seeing as I will have the chip mounted on one of those risers (cannot remember the name) so it is user replaceable, I do not think this will be a major issue.

see an earlier post, it seems my power board has a 100uF cap built in, I assume that works ok.

By this, do you mean you cannot read them, or you cannot see any issues?

All seems ok,I plan to order them around 3 today. Let me know if anything else looks bad.


That cap is to handle switching transients of the PowerBoost, I would have an additional cap on the board.

I’m not sure why you capacitively couple the RST pin but are you sure you don’t need a pull-up resistor on the pin?

I usually use 1K pull-ups on I2C lines.

Check that you don’t have pins 2 and 3 of the Powerboost reversed.

Yes, but it’s okay, if I save the image and then zoom in I can read it.

Anyway, hope this helps, good luck!


I caught the pull up right after seeing that. As for the cap, I have no clue, but everyone on the arduino forum does it, and the arduino has it too, so I will play it safe.

I will stick with the 4.7K for now, and switch them out if necessary, thats the advantage of THT parts

Don’t Think so. I have labeled them as the breadboard style, which is labeled differently than the schematic style (no clue why adafruit did that). Anyway it is doubtful that I will actually use that connection, it is just there for future-proofing.


Thanks for everyone’s help, I plan to make a post summing up what I learned, so knowledge can be passed on to other people.