How to verify that the pin designators in schematic symbol and footprint match? - Page 1
Forum section: electronics / general

author: matrixofdynamism
author_rank: Regular Contributor
timestamp: March 13, 2022, 11:56:13 pm
content: I am new to Altium and started with the video tutorial from Robert Feranec of Fedvel Academy. It is a great set of tutorials to get started.When I went into the PCB design stage, I found a set of "unknown pin" errors. I eventually found that this was because the pin designator (not pin name) for the diode component was named 1 and 2 in the schematic symbol but was named A and K in the schematic footprint. The problem went away when I modified the footprint symbol to use the same designators as the schematic symbol. The mismatch happened because I used the footprint wizard to create the schematic footprint of the diode.Now I have two questions:1. Is there a way to automatically check if the schematic symbol and the footprint match for a component?2. What exactly is the purpose of the "Validate PCB project ..." command? I had wrongly assumed that it would catch such errors.

author: twospoons
author_rank: Frequent Contributor
timestamp: March 14, 2022, 12:48:37 am
content: I would advise sticking with numerical pin numbers everywhere. There are many common packages, such as SOT-23, SC-70, SO-8 etc that are used for diodes, fets, bjts, ics. So the base footprint will use numerical pins to be compatible with everything. If you start using letters for pin designators then you have to create different footprints for diodes, fets, bjts etc, instead of having one common footprint.So keep the pindesignatornumeric and use the pinnamefor A,K etc.

author: free_electron
author_rank: Super Contributor
timestamp: March 14, 2022, 02:26:15 pm
content: A couple of tips (and this is not altium specific ! )The library is the most important part of the design process. it needs to be right. A library mistake has ramifications for everything you do and can create massive damage / delay.The following tips are based off 30+ years experience doing boards and dealing with mass production by hundred of companies and interfacing with a large number of other tools.- component names should be UPPERCASE alphanumerical only and no longer than roughly 20 characters. begin with a letter and use letter and numbers only. a - is permissible. other characters are NOT ! <interoperability>- every pin needs to have a unique number. UPPERCASE alphanumericals only no other characters allowed <interoperability>- pick a convention and stick to it. example : Pin 1 is always cathode (assuming pin 1 is in use of course) EVEN if this part sits reversed according to the datasheet ! normalise it. <management>- there is ONE SOT23 in the library. just like there is ONE 0805 resistor package (exceptions can be special landpatterns for sense resistors but those are called - ) <management><interoperability> : deviating from this rule gives problems when exporting data to other tools (simulation , odb++ , ipc2581 , netlisters and whatnot. these external tools can throw a fit on the data. this gives delays or sometimes plain wrong output. odb++ cannot handle duplicate pins. pin numbers need to be unique. same for pdn analysers. they trace back to pin number/package : pin 13 in U15 has a problem.. but there are to pin 13's U15 ... the software throws a fit !)<management> you want to keep the variations low. this allows for easy variant management and when you touch master data all parts get updated. this is a double edged sword ! But one-for-all has more advantages than the other way around. use best judgement.