Jaguar 0.4-alpha over voltage clamp trace routing mistake

[DeuceEFI]

Ok, so there are some issues with the footprints on the over voltage clamp circuit SMD footprints I used for the adjustable zener and the PNP transistor. I found these mistakes when I was testing the over-voltage protection circuits on my Jaguar 0.4-alpha board.

I have learned my lesson to make sure the KiCAD footprints match up to the datasheet for the components as not all SOT-23-3 and SOT-223 device pad numbers are the same.

ie: the KiCAD foot print for SOT-23-3:

Code: Select all

        ______
pad #1-|      |
       |      |- pad #2
pad #3-|      |
        ______

However the manufacturer datasheet for the adjustable zener shows the pinout for the SOT-23-3 as:

Code: Select all

        ______
pad #1-|      |
       |      |- pad #3
pad #2-|      |
        ______

There is a similar problem between the numbering of the pads for the SOT-223 PNP transistor (Q12).

Luckily this did not result in letting the "magic smoke" out of the components, they are OK so after you make a few modifications the over-voltage protection circuit will work properly:

Cut the 5 traces as indicated by the yellow lines.
Next connect the pads as indicated by the pink, orange, green and both blue lines on the drawing.

[superlen]

Bummer on the footprint Andy. That's burned many a pcb designer, myself included....repeatedly. So at least you know you have company and that it will happen again in the future.

Sometimes, you can just flip your part upside down, or upside down and rotate 120 degrees to at least get your prototype going. This works much better with sot23's than it does with sot-223s.

I finally made a rule at my company....ALL three terminal packages in the master pcb library are numbered 1,2,3 left to right. PEROID! Then you make the schematic part match the datasheet in *function* & disregard the pin #s in the datasheet, if they happen to be 1,3,2 which many are. What we found is that many times we had the schematic proper but the wrong flavor of footprint was being pulled from the pcb library as we had multiples pinouts represented. During design review it's easier to see the schematic error than it is to notice the footprint. We also made it mandatory that the pin *numbers* show up on the schematic & aren't hidden to make it cleaner. No E,C,B instead of pin numbers or G,S,D, ect. You can have those as additional information, but the numbers 1,2,3 better be on there. Couple that with the fact that you *know* the footprint is 1,2,3 L-R and it's easy to review with just the schematic and datasheet in front of you.

After a while all the parts in your library have been tested by fire, so when you grab one you know its proven which also helps....now lets hope I don't blow a footprint on my next layout and have to own up to it here. lol

Great job on the jaguar, BTW. I haven't looked at it in great detail yet, but from what I saw it has been well thought out and executed.

Lenny

[Fred]

I can see why you did that, but this is a bit different to a closed-source gig: People have to read the datasheets and read the schematics and make sense of it. I'd be strongly opposed to seeing pin numbering not match the data sheet, either in lib, schem, or pcb for that reason. I think it just comes down to taking care while creating the part definition and not making any assumptions. And I reckon this holds true:

A lesson hard learned is not quickly forgotten.

IE, that melted CPU wasn't cheap, it won't happen again :-) (And next testing will be before the CPU goes in, I guess.)

Fred.

[superlen]

Good point on the open source confusion factor. I can see were if the schematic is showing one pinout and the datasheet is another, someones going to be thinking WTF. Of course it would have to be the part that takes out the micro instead of some transistor driving an led or something cheap.

I had a production pcb under test that was designed to monitor/control large three phase gensets. It had mains power of course during the test and was programmed and tested via a usb programmer. We had built 1000's of these boards with no problems, however one came through with a solder bridge in just the right spot & took out the micro, the usb programmer & the motherboard (via usb) on the test pc. Argh! It just happens sometimes.

Len

[Fred]

Ouch, bad luck! I stuck my headphones into the USB socket on my macbook air one night in the dark and killed the machine. It came right back up, though. Direct short of 5V isn't processor/memory retention happy ;-)