I created my first PCB design - its a remix of PCB I found already on the market with some added 12 V DC jacks and XH-2A jack - this will only ever be used with 12 V up to 2 A - wondering if there are any mistakes I made or things I need to be careful of - don’t want anything to go wrong.

enter image description here

enter image description here

enter image description here

enter image description here

  • \$\begingroup\$ Welcome and congratulations! Please put a ~10 ohm gate resistor on each MOSFET. \$\endgroup\$
    – winny
    Commented Aug 23, 2023 at 15:04
  • 1
    \$\begingroup\$ Just a comment: a "U" reference designator is usually used for ICs. Connectors are usually "J". \$\endgroup\$ Commented Aug 23, 2023 at 15:25
  • \$\begingroup\$ Did you verify your solder mask layering on it's own?, (try turning off all other layers except solder mask and edges/outlines then review). Seems that in your second picture the pads for R1,R2,R3 show a different layering pattern (colors) as compared to all the other component pads. \$\endgroup\$
    – Nedd
    Commented Aug 23, 2023 at 18:07
  • \$\begingroup\$ You are using slots for the DC jacks. You can use round holes, it will be cheaper to fabricate the PCB this way. Alternately, there are SMT versions of these jacks. \$\endgroup\$
    – Lior Bilia
    Commented Aug 23, 2023 at 18:28

1 Answer 1


Generally pretty good!

You might want to confine your use of wide traces and multiple vias to nets that actually require it, and add thermal reliefs to things like the SMT resistors and LED. It will make hand soldering more difficult and might cause tombstoning in reflow (in the latter case, you want the pads to be thermally similar).

You also might want to have a thermal break between the two MOSFETs so the one carrying more current can get relatively hotter. Maybe even a routed slot.

You should have polarity marking for the LED on the silk screen layer. Maybe a part number and revision number somewhere.

You might want to leave a bigger clearance around the mounting holes, there's really no reason not to.

Hopefully a low-side switch is appropriate for the intended application. It can sometimes cause issues, particularly if there are alternate paths for current.

It's a very simple circuit and I don't see anything wrong with it, except CN1 appears to be reversed compared to the schematic (square pad pin 1 is input and pin 2 is ground).


Your Answer

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

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