From the point of view of the land pattern it doesn’t matter whether cathode is pin 1 or pin 2 as far as the footprint pin numbers match the symbol pin numbers.
It could matter the silkscreen because it usually marks the cathode.
I think labumm believes that the most positive connection to the Zener diode (in the circuit) is “anode”.
That’s not the case: anode and cathode are always the same, regardless of diode type.
I see no errors in the documentation anywhere.
The large pad is anode. period.
I have it in the circuit and measured it.
The discussion here lead me to find the actual mistake. A rookie mistake. The pin numbers on the symbol I was using don’t match the pin numbers on the footprint. When I found and corrected the mistake in the physical pcb I went to the vishay data sheet. The data sheet doesn’t have pin numbers. Evidently the anode/cathode pin numbers are not standardized either. I suspect I dropped in the generic library symbol (D_Zener) and then later linked the symbol tothe footprint of the part I selected. I was blaming the wrong mis-match.
The cathode is the small pad, as you correctly point out.
And, this is why I prefer having symbols with pin letters instead of numbers - A & K vs 1 & 2…
I will give this discussion a certifiable “WOW.” I have a good collection of Vishay diode datasheets, and I found this one easily (Vishay # SS2P5 and SS2P6)
1 Like
If you have big collection then you can check if it is random or it depends on diode type.
May be Schottky needs bigger cathode while Zener anode.
The question is if it is better to have transistor symbols with all 1,2,3 combinations or to have each transistor footprint (SOT23, SOT323, SOT89, SOT223, DPAK,…) with all B,E,C and G,S,D combinations.
Yes, and this horse has been beaten quite a bit here.
I prefer the later, since it means I don’t have to change the schematic if I substitute a transistor. But, I am used to a decoupled BOM.
TPSMP series TVS diodes (basically Zener with high peak power dissipation) TPSMP datasheet have “reversed” polarity, while all standard SMP diodes have the standard “cathode on the big pad” polarity (AU1P series, MSE1P series, SS3P series)
It appears that if it comes to diodes in SMP packages Zeners have a different pinout to standard diodes.
Above is the mouser data in the SS2P5. I checked the D_Zener, 1N4001, LED, and D_Schottky in KiCAD. They all have K=1, A=2. The spec sheets don’t assign pin numbers.
The generic KiCAD symbols also label the pins, so the K and A assignment from the symbol come through to the PCB footprint. See below. The generic D_Schottky with as-imported footprint from SamacSys. It’s backwards.
Which is the most common way to number K and A?
For KiCad and most PCB design software it’s 1 - Cathode, 2 - Anode
For SPICE simulation software it’s 2 - Cathode, 1 - Anode
1 Like
I guess it doesn’t help that pin numbers on KiCad’s default diode symbol are hidden from view, here’s a pin table for “Device:D”
How do you pull up the pin table? I can get to something like that from: symbol properties>Alternate pin assignments
What this means is that there are two flavors of diodes D_KA and D_AK that need to be tracked. Or converted to the KiCAD standard D_KA for use. That adds a layer of abstraction connecting the symbol to the footprint.
Is this also the case for polarized caps?
For polarized caps in KiCad’s library it’s 1 for the positive and 2 for the negative.
I typically use a separate footprint for these “reversed” diodes since the silkscreen marking for the cathode band would also be on the opposite side, and then assign a correct variant of the SMP footprint to the diode symbol. Standard SMP footprint on the top and “reversed” SMP footprint on the bottom.
That way they can be both used with the generic diode symbol.
1 Like
I queried SamacSys as to their pin assignment standard. They replied, “Ordinarily we use K for pin 1, so I will make sure this is reiterated to the builder of this part.”
And it’s fixed.
1 Like
Wait a minute… I had not heard of SamacSys…but that much is OK.
Why does the symbol show pin 1 on the left and the footprint shows pin 2 on the left? I don’t think there is any sort of “rotation convention” in effect here, so the symbol and footprint ought to be rotated the same way, right?
On SS2P5 and SS2P6 the cathode is the larger terminal, but the SamacSys drawing appears to be worng.
oops, not fixed. They swapped the pins on the symbol only, so not it really wrong.
Inthe pop up display, they don’t have the symbol and footprint oriented the same way. It’s not wrong, but poor practice as it is easy to misread.
SamacSys is the group that does footprints for Mouser. Honestly, now that I have a bit more experience with SMD and KiCAD, I think I’ll just use the KiCAD footprints.
1 Like
That sounds good. I sometimes refer to the KiCad footprints but I generally make my own for easy hand soldering.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.