Electronics > KiCad

Is it me or is the symbol/footprint mapping in KiCAD kind of wacky?

<< < (3/3)

free_electron:

--- Quote from: Doctorandus_P on July 18, 2024, 12:17:33 am ---1. Put all pin numbers in the schematic (Yes, this is done sometimes, 4 pins connected to the drain...

--- End quote ---
That is the right way to do it. the only right way. ( i will explain later)

--- Quote ---2. Use pin stacking. this hides the pins in the schematic, and I don't like it much.

--- End quote ---
do not hide things in the schematic ! stacking is no-no


--- Quote ---3. Just give the pads in the footprint the same number.

--- End quote ---
ABSOLUTELY NOT !

Here is the reason :
if you ever will have to deal with external tools that act on the PCB layout data (flying probe or bed-of-nails testers, ipc netlists, odb++, factory floor software, field / thermal / pdn analysis l ) every pad needs to be uniquely identifyable. Power domain analysis : pin 1 has a lot of current. There's 4 .. which one ? The tools can't resolve.
odb++ will add suffixes to duplicate pin numbers which means you cannot re-import processed data. it breaks the netlist. so the testers cannot resolve the schematic netlist vs the pcb netlist : the names have changed !
It creates and endless headache. You do not know where and how your data is post-processed.

non-functional pads ( mounting holes, unplated or plated ) need to be given a unique designator that is NOT numerical. don't make a 10 pin connector with two mounting holes called 11 and 12. If there is a mismatch between symbol and library the tools will never catch it Give them a unique name MEx ( Mechanical x) . be consistent so that you can filter on those pads and set rules for them ( soldermask retraction , clearances etc )

Note that the above is not KiCad specific. I Was searching for something else on the forum and found this post so i reacted.

Navigation

[0] Message Index

[*] Previous page