When trying to update my pcb in pcb editor I get an error stating that a pin that is shown in my schematic symbol is not found in footprints. Does anyone have a resolution?
Thus far I tried to re-label the pin’s name (changing the name to MP in footprint editor) so it can better match the schematic and that didn’t work.
I am new to this and any help is much appreciated!
Looks like you’re in over your head. Your should follow the instructions here to promote your level to be able to post a zip of the project. I think there will be multiple problems with it.
And also paste the complete version information from Help.
Your Symbol and Footprint associated with that Symbol have to have the same number of pins . . . do they ?
Are you using a footprint with a pad named “MP” or “1”? And does it match the symbol pin name (which seems to be “MP”)?
Most KiCad stock test point footprints have the pad numbered “1” e.g. TestPoint.pretty/TestPoint_THTPad_1.0x1.0mm_Drill0.5mm.kicad_mod · master · KiCad / KiCad Libraries / KiCad Footprints · GitLab
They have to be the same. It’s easiest to change it in the schematic if it’s the wrong symbol. In fact based on the ref des prefix being “H”, I think you have used a mounting hole symbol, not a test point symbol (which is usually “TP”).
As johnbeard mentioned your (probably default) footprint TestPoint_THTPad_1.0x1.0mm_Drill0.5mm has a pad number 1. KiCad does have a symbol with the name MountingHole_Pad_MP and this does have a pad with the name MP. You have so many of these footprints, that it is not likely you are using them as mounting holes. the hole of 0.5mm is also a bit small for that.
I suggest you use: Schematic Editor / Edit Symbol Library Links and then replace all these “mounting holes” with TestPoint or TestPoint_Small symbols. You can also do this by first opening the properties of one such symbol and then use Change Symbol from it’s properties window.
In the end, it’s only important that the pin numbers in the symbols use the same ascii string as the pad numbers in the footprints. On itself MP is a perfectly valid pin “number”, and I’m not sure why it did not work for you. Labels are case sensitive, I’m not sure whether pin / pad “numbers” are case sensitive. A short search though the manual did not clarify this either. Another possible cause is that you did not run Update PCB from Schematic [F8] after you changed the footprints, or maybe you only changed one footprint?
It is also much easier to experiment on a small dummy project. You don’t get drowned in a gazillion error messages, and if you make some serious mistakes, you just trow away the dummy project and make a new one. This removes all the stress of getting an important project “right”, and you can focus on learning KiCad instead.
If you still have problems after all this advise, then:
If we can look at a (dummy) project, it’s often the most direct and quickest way to diagnose a problem.
It is not clear what you were editing.
Symbols (at schematic) have pins and pins have Name and Number.
Footprint (at PCB) have pads and pads have Number.
Numbers have to be the same to let KiCad link pin at schematic with pad at PCB.
You couldn’t edit name in footprint editor, or I don’t know something.
If you were using footprint editor it is also not clear if editing/modifying footprint at PCB or editing footprint in library.
Yes that’s my guess too, OP used mounting hole symbols instead of test point symbols. I’ll also guess that OP was tasked or decided to add test points to an existing design.
