Lots of warnings "Pins of type Passive and Unspecified are connected" - due to import?

Schematic
1

Yes, this project is based on an EasyEDA import.
I have also lots of “pins of type power input and unspecified …” and passive and unspecified.
I have replaced all symbols (and footprints) with KiCad parts.
ERC returns hundreds of warnings like:

image
image1108×271 47.4 KB

Please help me sort it out. There are no errors, only warnings.
full list attached.
ERC.rpt (44.1 KB)

2

It looks like the interpretation of “unspecified” pin types between EasyEDA and KiCad is different. In KiCad, you can not connect anything to an “Unspecified” pin, while apparently in EasyEDA you can connect anything to an unspecified pin.

If there is really such a difference in interpretation of the “unspecified” pin type, then this probably should be fixed in the EasyEDA importer.

Other options are:

  1. Replace the imported symbols (LED’s, switches, maybe more) with native KiCad symbols.
  2. Suppress ERC warnings for the “Unspecified” pin type in this project.
  3. Change the error matrix (Schematic Editor / File / Schematic Setup / Electrical Rules / Pin Conflicts Map) for this project.
3

Undefined in EasyEDA → Unspecified in KiCad is the best match, so I don’t think there’s an issue with the importer.

image

You can change severity in Schematic Editor / File / Schematic Setup / Electrical Rules / Pin Conflicts Map, or change pin types in symbols according to your schematic.

4

can I rather correct this somehow? - maybe text search/replace?
I’d rather fix this properly so it does not pop up in the future.
@dsa-t suggested:

  1. Replace the imported symbols (LED’s, switches, maybe more) with native KiCad symbols.

I already did, all symbols should be replaced, or maybe there is very few left like 0-3.

This, for example is “Device:Resonator_Small” - and it still gets the arrows:
image

those are Device:C and power:GND - and then tere are arrows between.
image

maybe “change symbol” retains some bad data?

5

Textually it is is apparently a close match, but functionally it is not. Apparently EasyEDA uses these pins for LED’s and Switches.

I also already mentioned the Pin Conflicts Map:

image
image1020×523 71.7 KB

In KiCad, pins that can be connected to “anything” (because it’s impossible to know in advance (in the library) how the symbol is going to be used are marked as “Passive” in KiCad. This includes resistors, capacitors, BJT’s, Source and Drain of FET’s (gate is sometimes an Input, sometimes it’s passive too) Buttons, switches, encoders.

I am not familiar with EasyEDA myself, but as it’s web based, I just opened an example project and edited a resistor. ERC seems to be very limited with just the pin types

  • Undefined
  • Input
  • Output
  • I/O
  • Power

image
image866×573 46.6 KB

And the manual confirms this (Search for: “Electric”)
https://docs.easyeda.com/en/SchematicLib/SchLib-Attributes/

In this context, it does not make sense to map any of the EasyEDA pins to “Unspecified”, and mapping “Undefined” to KiCad’s “Passive” is more appropriate.

6

we posted at the same time :slight_smile:
but the main question stands: how to clean it up?
as you see above, changing symbols does not seem to fix it.
Here: replaced LED symbol, deleted wire, deleted GND, added new GND - and the issue remains.

At this time I did put a bunch of work into this schematic, and it is too late for a new import.
But I hope to somehow be able to fix it, even it it is text-replace in the schematic file.

7

That has already been mentioned both by me and by dsa-t. It does not seem very useful to repeat that.

8

I see the following suggestions:

This is not solving the issue, but hiding it. I am reluctant to just start disabling/inhibiting checks.

Then I see those three suggestions:

#1 is what I tried and it did not work - see above.
#2,3 is still hiding the issue, rather than fixing it. with opportunity for future problems.

Please suggest a way to actually fix it. (change the pin types) without deleting and replacing every part.
Additional info: for this LED, both pins are “passive” - the GND symbol is new… the wire was deleted and redrawn… and issue remains.

9

Found it ! - it was ONE bad component symbol that was connected to GND that caused all those issues.

10

Now you see why foreign symbols and footprints have a bad rap, at least in my book.

1 Like
11

I find that a bit of exaggeration. The issue itself is easy to fix, and the problems are mostly due to inexperience with KiCad.

I tend to make my own symbols and footprints when needed, but if they are easy to find on the 'net it can save you some time. I would never trust such parts (especially pin names, pin numbers, and then footprint pad numbers and pad locations) but you should verify all that regardless of what the source of your data is.