Is my Schottky diode symbol reversed in my F.Fab layer? [solved]


Hello everyone,

I was just reviewing my first pcb I want to send off for production and noticed that the schottky diode symbol on the f.fab layer looked reversed to me. I wouldn’t call myself an expert on electronics so I wanted to double check here. Is the symbol on the F.Fab layer reversed? The blue arrow indicates the flow of electricity from the usb power supply and the yellow arrow indicates the flow of electricity to the rest of the board.

A little confused here :slight_smile:


The symbol on the F.Fab is not reversed. The pin numbers in the schematic symbol are reversed.
Usually, cathode is pin 1 and anode is pin 2.

From the kicad point of view, it doesn’t matter which pin is number 1 or 2. What is important is the pin matching between schematic symbol and footprint. Both direct or both reversed.
In your case it seems that pins don’t match.


My instinct is to say that the pin numbers on your schematic symbol are backwards. The industry standard for diodes is to have pin1 on the cathode. Your symbol has pin2 on the cathode.


My guess is you took a symbol meant for simulation instead of one meant for pcb design. Sadly spice choose a different pin numbering scheme to the pcb design world (back when these decisions were made nobody imagined that the same software solution will ever be used for pcb design and simulation.)

Notice the pin and pad numbers of your footprint and symbol. KiCad uses these to decide which symbol pin represents which footprint pad: How does KiCad know which symbol pin represents which pad of the footprint?


Thank you for pointing this out! Very possible, I made the schematic symbol myself. And I think I fiddled around with the footprint pins as well as I was confused about the issue.

I am afraid I am to blame for this as I made the symbol myself :sweat_smile:
However I am happy you guys pointed this out. I won’t make this error in the future :smiley:

So I changed the symbol in my schematic to the kicad schottky diode one (which I could not find for some reason when I was still making the schematic a couple weeks ago. I was still very new to KiCad at that time). This is how it looks like now.

So from what I understand you guys suggest I should replace the currently connected footprint to the one on the left as the suggested net lines indicate right?

Please let me know!
And thanks for the help :smiley:


That is the basic idea. Delete the “old” footprint for D4 and park the “new” footprint in its place. (The existing traces may be OK as they sit . . . or you may have to shift the trace connecting to C8 by 10 or 15 mils toward the top of the image.) Verify that your netlist is up-to-date. (Looks like you have already done this.) Offer up sacrifices, rituals, and prayers to the appropriate deities. Click the “Run DRC” selection . . . . and . . . . SHAZAM! Your design passes with no DRC squawks!

If you have defined the drawing origins for the footprints at the geometric center of the part, the “Properties” of the “old” footprint contain the X-Y coordinates that you can copy over to the “new” footprint before deleting the “old” footprint.



I did just that! Thank you guys very much for clarifying and helping me out here! I am very glad I spotted this mistake before sending the gerbers over for production :slight_smile:


I’ve been burnt with this pin numbering reversal due to how the schematic symbol and footprint library models were created earlier. Since then, I made it a point to make sure I edit the symbols and footprints both to use “A” (for ANODE) and “K” for (CATHODE) as PIN NUMBERS. Yes, the pin numbers don’t really have to be Numbers - you can assign alphabetic characters. That makes it very unambiguous.


Only problem with that is that you now need a sot23 footprint for a diode, one for a transistor, …
As footprints are much more closely tied to manufacturing i rather have only one footprint per physical package and make the correct connection via fully specified symbols.


Using A and K could be awkward if you use a third party board assembly house as they expect pin 1.


Concur. I only use if for 2 pin polarized parts


Haven’t had problems till date. Although, I’ve only used Seeed Studio, so not sure if other board houses will complain.


This is not an issue for the PCB maker. It affects the assembly houses that have to program pick and place machines. The component reels define pin “1”, not k etc


Ah, gotcha. Seeed have been assembling all of my boards, and haven’t messed up yet. So I’m not complaining :slight_smile: