I’m guessing that @topherbuckley hasn’t noticed that in the device library the commonly used jelly bean symbols are already just a single character. Specifically to make it faster to find and place symbols. Entering only D in the filter gets the schematic diode that he wants, R is resistor, C is capacitor, CP is polarized capacitor, L is inductor. Yeah that last one looks weird until one realizes that “L” is the traditional reference designator letter for inductors. Recognizing the pattern set by that last one it makes sense that Q gets transistors…
Every industry has its own jargon, and learning the jargon is the first part of mastering the industry.
I did. That is precisely why I proposed the change to pspice.D. As such, the Device.D still take precedence in the filter/sort for input of ‘D’, thus making the pspice.D component a non-default symbol for both a search of ‘D’ and ‘DIODE’.
I didn’t see an answer above about why the generic diode symbol has the pins opposite the simulation diode symbol. And I know the answer.
The SPICE diode primitive has the anode as pin 1, so it’s by far easier to use that convention in the symbols. Otherwise most diode models would need to have the pin numbers swapped. That’s a hassle that the users can avoid if the simulation diode symbol pinout is best suited for the simulation tool.
IPC says that the cathode is pin 1. Opposite of the above. And so all other diode symbols stick with this industry-standard pinout.
The SPICE diode issue could be fixed very easily if the library maintainers understood how or wanted to: In V5, add the following (or appropriately adapted) line to every diode library symbol (except to SPICE symbols that have the pins swapped already):
@franzee Thanks for the constructive post. Can you explain this in context to a spice and non-spice library symbol and how it would work as you claim? I’d have to look through the ngspic docs again in detail to parse the syntax. Could you do the rest of us laymen a favor and explain a bit more what this is doing? I’ll forward this onto an ongoing thread on the symbol library gitlab repo if it makes sense.
@topherbuckley It’s a KiCad feature that allows to re-order pins for simulation netlists.
SPICE has a well defined pin or node order for the built-in circuit elements: 1/+/A, 2/−/K, etc., and by default symbol pins in KiCad are mapped in the same order to SPICE pins.
The Spice_Node_Sequence property above corresponds to the Alternate node sequence field in the Spice Model Editor (Edit Spice Model… button in the Symbol Properties). It’s empty for capacitors, resistors and inductors because the default is correct or doesn’t matter. For diodes, KiCad symbols adopted K (cathode or −) as pin 1 and A (anode or +) as pin 2 as a convention, and footprints rely on this (that’s why the PSPICE diode symbol with the swapped pins can only be used for simulations).
Adding 2 1 as a node sequence remaps the pins for simulation only, and footprints are not affected. If this would be done for all 2-pin diodes, they could be used for simulation also. (Unfortunately, there is also a bug in that it remaps the order in which pins are defined in the symbol instead of their number, but since usually pin 1 is defined before pin 2 it works.)
