I printed my first PCB. When I received the board, I realized that the status LEDs are not working. It seems like they are reversed. I double-checked the design and the schematics seem to be correct but the PCB design doesn't follow the schematics - unless I am missing something.

I am using EasyEDA application for the design.

In the first image, I have an array of LEDs where the top connections are 5 V going to the LED anodes then to a resistor and then finally to ground.

The automatically-generated PCB design (seen in the second image) seems to have the anode and cathode of the LED swapped. The yellow arrow on the LED indicates the anode-to-cathode direction.

Am I missing something here or is this a bug in the software?



  • \$\begingroup\$ EasyEDA seems to have an infamous history for diode footprints (even those in the official library) with some of them having anode and cathode swapped. (Saying this as of 2020ish experience.) For (fictional) example, while the 0603 LED might be the correct way around, the 0805 LED might be wrong. That was really messy. Other than that, their officially maintained footprints have usually been of excellent quality. \$\endgroup\$
    – tobalt
    Feb 1, 2023 at 9:41
  • \$\begingroup\$ @tobalt In all fairness this seems to be a recurring problem with many tools and component libs. In my experience, the most common assembly-related quality problem with prototype boards is that all LEDs got mounted backwards. Either because of a bad symbol or because of a lack of polarity markings. \$\endgroup\$
    – Lundin
    Feb 1, 2023 at 9:46
  • \$\begingroup\$ @Lundin EasyEDA was my first EDA tool ever, and it was the one where I learnt about this stuff, luckily before making boards. Ever since, I double check and I am extra explicit (aka double dummy safe) when communicating with assemblers. \$\endgroup\$
    – tobalt
    Feb 1, 2023 at 9:47

2 Answers 2


Indeed it would seem that this particular component in the library is broken. The "half cross" symbol should "point" towards the cathode. Similarly a triangle symbol is sometimes used, pointing to the cathode. So your PCB CAD has placed the diode backwards in the layout vs how it was defined in the schematic.

Probably not a "bug" but a bad component in the library.

  • \$\begingroup\$ tldr; I got bamboozled. Will try to flip them manually. I guess I need a heat gun? \$\endgroup\$ Feb 1, 2023 at 10:21
  • 2
    \$\begingroup\$ @ArtursVancans Since they are LEDs, I would just desolder them using your favourite method, throw them in electronics recycling and mount new ones. LEDs don't like to get heated up multiple times. And the "heat gun" if used has to be a desoldering station, not some generic heat gun you use for shrink tube and the like. You should be able to remove these with a soldering iron though. \$\endgroup\$
    – Lundin
    Feb 1, 2023 at 10:23
  • \$\begingroup\$ @ArtursVancans Those LEDs look small enough (0603?) you can very easily remove them with a regular soldering iron. Just heat one side and gently push it off the pad (it'll pivot around the cold pad) then heat the other side to detach it completely. Do it slowly to avoid damaging the second pad. It's super easy and then you can resolder it the right way or replace it (I agree with Lundin, it's easy to damage those with the iron). \$\endgroup\$
    – TypeIA
    Feb 1, 2023 at 23:08
  • \$\begingroup\$ @TypeIA Thanks. I managed to flip most of them (15 in total). Broke pads for 2 unfortunately, but it's ok. \$\endgroup\$ Feb 7, 2023 at 5:40

LED polarity is a notorious source for errors in PCB assembly.

There simply isn't any standard on LED polarity. That "half cross" symbol for example may point towards the cathode or the anode depending on the manufacturer. There are even manufacturers that have both variants in their portfolio!

If something can be remotely considered "standard" than it's the cathode being the "special" pin that is marked on way or the other. But you certainly can't rely on it!

So you can't even argue that the part in the library is broken. Maybe it is, but after all it's just one way of indicating LED polarity. The library should at least be consistent, of course.

With LEDs in third party libraries you should always, always always double check on how the schematic symbol translates to the footprint and to check the LED's datasheet on how the manufacturer is indicating the polarity on the package.

A good library is ridiculously distinct about LED polarity. This means there is a diode symbol on the layer that is used for the assembly drawing, for example. And there is a diode symbol (or a triangle) or at least a cathode marking on the silkscreen when there is enough room on the board. Also the pads should be named "K" (or "C") and "A" instead of "+", "-", "1" or "2", if supported by the ECAD tool.


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.