I am relatively new to SMD parts. I am using a 5.6V zener (Vishay PTV5.6B-M3/84A) which uses a DO-220AA footprint. When I got the boards back I noticed the footprint pads were swapped (one is big ad the other small) and did not agree with the cathode mark/band. I thought I just screwed up, but looking at the spec for the diode and then the generic DO-220AA I see the footprint assigned both ways.
Is there are standard where normal diodes are one way and zeners are the other? Or is this just random.
I believe itâs just random. DO-220AA standard does not specify which side should be the cathode, and typically zener diodes have the same polarity as standard diodes in comparable packages. It seems that this specific diode is just special in that regard. The datasheet you attatched confirms that the cathode is the smaller pad on page 4.
Itâs probably related to the physical construction of the PN junction inside, typically cathode has a bigger surface area and is used as a primary heat sink but in this case itâs the opposite.
Thanks, that makes sense. What I find disappointing is the the footprint on Mouser, is backwards. Thatâs were I got it. I have gotten several bad footprints from SamacSys. The symbols are usually unhelpful. Fortunately I tend to design with a few dozen parts,so thatâs not so hard once I have my library set up.
My original statement âItâs not fixed yet. That footprint is wrong. Pin 2 (cathode) is the large pad.â is wrong, see below.
From the Visahy data sheet linked above.
Since beginning of this thread I donât see where is a bug you are trying to show.
Based on what you draw a conclusion that cathode is the large pad?
At each of 4 Vishay pictures the big pin/pad is at left and small at right and the Cathode Band is clearly at right so according to datasheet cathode is the small pad.
I start to suppose that may be what you want to say is that you have that diode and measured it and from it you know that cathode is the large pad. If it is what you want to say than you havenât made it clear so far.
All pictures I have seen in this thread and in linked datasheets tells me that cathode is the small pad.
From the point of view of the land pattern it doesnât 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 âanodeâ.
Thatâs 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.
The discussion here lead me to find the actual mistake. A rookie mistake. The pin numbers on the symbol I was using donât 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 doesnât 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.
I will give this discussion a certifiable âWOW.â I have a good collection of Vishay diode datasheets, and I found this one easily (Vishay # SS2P5 and SS2P6)
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,âŚ) 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 donât 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 âreversedâ polarity, while all standard SMP diodes have the standard âcathode on the big padâ 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 donât 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. Itâs backwards.
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.
