Electronics > KiCad

Kicad, what does this unconnected paste error mean?

(1/1)

PartialDischarge:
I'm using a BGA footprint (Housings_BGA:Texas_DSBGA-6_2x3_0.9x1.4mm_Pitch0.5mm), and the PCB gives the following errors.
However the board is fine, with holes for the stencil...

Doctorandus_P:
It is an error in the Footprint itself.

In KiCad it is legal, (and common) to have multiple pads with the same pad number to make big or complex pads. For examples for this, search through KICad's Footprint libraries for any footprint with "thermal" in it's name.

Your situation is different though. For most footprints, the shape of the paste and mask layers is derived from the pad itself. For some footprints though, the solder paste or mask have a different shape, and in such cases a different pad is used, but with it's copper layer turned off. I believe these are called "aperture pads" in KiCad. These pads are however not allowed to have a pin number. The pin number string must be empty, and this is not the case in your footprint.

You are also using quite old libraries. The plural form of Housings is a strong indication that this is a library for KiCad V4.
The closest match I could find in a KiCad V5 library is:
>  Package_BGA:Texas_DSBGA-6_0.9x1.4mm_Layout2x3_P0.5mm

And in this footprint the error is corrected. The pads for the F.Paste layer does not have pin numbers.

So the next question is:
Are you aware you are using an old library or has this just slipped your attention?

This may be relevant for you:
https://forum.kicad.info/t/i-had-kicad-4-installed-previosly-now-i-updated-to-v5-now-i-have-some-problems-with-the-library-setup/11932

PartialDischarge:
I'm using Kicad 5.1.9 for MacOS and I don't have that Package_BGA library, but a lot of Housing_*

According to the link you posted, I have the KIGITHUB variable as https://github.com/KiCad so it seems that I have version 4 of the libraries.

I have to decide what do I do since I have lots of boards designed with them already....

Doctorandus_P:
In KiCad, al used footprints are embedded in the PCB file itself, so updating your library setup should have no impact on already existing projects.
(For schematic symbols it's quite a different story in KiCad V5, they only link to the libraries).

There are also quite a lot of side projects around KiCad. Including the half-baked ones here is a list of about 60 of such projects:
https://github.com/xesscorp/kicad-3rd-party-tools

This one may be useful to you:
https://github.com/MitjaNemec/Kicad_action_plugins/tree/master/archive_project

But at this moment...
I'd consider to wait a bit longer before updating.
KiCad V6 is expected to be released somewhere this year and it has about 3 years worth of improvements over V5.

Navigation

[0] Message Index