I'm building a clock I found on Thingiverse. The designer created a custom PCB to connect three stepper motors, an Arduino Nano and some Hall sensors. Unfortunately there aren't many instructions. I've soldered up all of it minus one spot I'm unclear on. I've circled it in the image below (front and back from some extra boards):

enter image description here

What exactly would go here? A resistor? Something else? In a youtube video, he has a different version, but around the 4.56 mark, you can see the design and it's labeled as C2 10uf, not sure what that means. Any ideas?

  • \$\begingroup\$ it looks like it could be an option jumper ... are the two pads shorted together right now? \$\endgroup\$
    – jsotola
    May 27 at 20:47
  • 1
    \$\begingroup\$ @jsotola They're not shorted together in the Gerber; the pour and its haphazardly set clearance just make it look like it might be. \$\endgroup\$
    – nanofarad
    May 27 at 20:48
  • \$\begingroup\$ (Have you come up with why 12 "motor terminals" might be driven using 3 7-transistor arrays?) \$\endgroup\$
    – greybeard
    May 27 at 20:49
  • 1
    \$\begingroup\$ This is a really bizarrely laid-out PCB. \$\endgroup\$
    – Hearth
    May 27 at 20:53
  • 2
    \$\begingroup\$ Pcbs are cheap and there’s free software so everyone is a pcb designer! We need some AI to rate designs. \$\endgroup\$
    – Kartman
    May 28 at 1:32

2 Answers 2


The indication "C2 10uF" almost certainly refers to a 10 microfarad (uF) ceramic capacitor. The linked documents didn't include a bill of materials, but the bill of materials would generally be the place to look for details on the parts that should be assembled onto the board.

Also, the positioning of the capacitor is rather weird; IMO the designer should have placed the cap closer to the power supply pin it's routed to. Between this and other inconsistencies (as well as the lack of a bill of materials), I'm not very confident that the project's author paid enough attention to a quality circuit board design. However, with the boards already fabricated, there's not much you can do about that, and this design will probably work well enough anyway.

I ended up downloading the PCB files and measuring the pads of the capacitor using the gerber viewer tool bundled in my KiCAD installation - the dimensions of the pad seem to line up pretty closely with the standard "0805" surface-mount capacitor package.

Finally, the design seems to be using 5 V throughout for power meaning the capacitor needs to be rated to withstand 5 V; putting everything together, this means that you'll need a capacitor that has the following specs:

  • 10 microfarad (uF) capacitance
  • 0805 package (0603 is probably "close enough" but smaller and harder to solder)
  • Voltage rating of at least 5 V, but preferably more for a bit of breathing room. 6.3 V, or even 10 V, is a decent choice.

In this case, you did manage to find hints regarding C2 from the video. However, if you didn't have any such clues, you could trace the connections from the pads and find that they connect to the power supply line (at the barrel jack and Arduino VIN) and ground pour; this suggests that the part is a capacitor (since it's placed across the power supply near a chip, and capacitors are used in such a way to provide power supply decoupling).

Anyway, while I have this board up in a viewer, a few improvements that you could make if you designed your own board:

  • Tying 5V to arduino Vin will cause the Arduino 5V supply to sag below 5 V, because of dropout in the arduino's voltage regulator
  • All of the ICs should have similar capacitors across their supply lines, close to their supply pins
  • The board design looks careless overall, and could be made neater with careful hand layout.
  • There are no reference designators or corresponding bill of materials. If I needed to distinguish between multiple ULN2003N ICs, I'd rather be able to say U1/U2/U3, rather than "the middle one".
  • The current design has very few markings regarding polarity or pins for the barrel jack and motor connectors
  • 2
    \$\begingroup\$ It's so badly placed that I suspect it was just thrown together and then autorouted without further tweaking. Also makes you wonder why only one of the ULN2003Ns have it. \$\endgroup\$
    – pipe
    May 27 at 20:41
  • 1
    \$\begingroup\$ Thank you for such a detailed answer! That all makes sense now. I appreciate the effort you put in to the answer! Thank you again! @pipe - what is the downside of only using 1 vs 1 each for this particular use case? (sorry I'm more software than hardware :) ). \$\endgroup\$
    – yhax
    May 27 at 21:12
  • 1
    \$\begingroup\$ @yhax You want the capacitor to be close to each chip (with low inductance and resistance between the capacitor and the chip) - to do this, we tend to place the capacitor right by the power input pin of the chip. Consequently, we need one for each chip - if you had just one you could get it close to one chip but not the others. Sometimes, you'll also find a bulk capacitor for the board as a whole, usually near the power input or in some other convenient location. \$\endgroup\$
    – nanofarad
    May 27 at 21:20
  • \$\begingroup\$ makes sense, thank you for following up. \$\endgroup\$
    – yhax
    May 27 at 21:41
  • 1
    \$\begingroup\$ 10uF seems a bit high for a decoupling cap. The author- I hesitate to refer to him as designer- of the circuit probably knew that paralleled caps added, but didn't appreciate that they should be as close as possible to the chip to reduce the track inductance. And checking the layout might have shown up the spelling mistake... \$\endgroup\$ May 28 at 12:21

If you follow the traces on both sides of the board, you will see that one pin of the component (almost certainly a capacitor) goes to one of the power connector pins and the "Common" pin on all three ULN2003's (pin 9), plus the Vcc pin of the uC.

All spikes generated by commutating the motor phases are routed through the 2003 to this Common pin. You park a large cap on this net to absorb the spikes so they do not upset operation of the uC.

Personally, I would add another cap between uC pins 1 and 2 for additional, high-speed decoupling, something in the 1 uF - 10 uF range. SMT ceramic would be best, but anything that is non-electrolytic will improve noise immunity if you keep the leads as short as possible.


Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge that you have read and understand our privacy policy and code of conduct.

Not the answer you're looking for? Browse other questions tagged or ask your own question.