Assign net name automatically to footprints value

[ekoeck]

Hey there. I have a component called “test point” which has only one pin and as footprint just a small copper circle without solder mask. Additionally its value and a small dot is on another layer so that I have an overview of all test points for my documentation which looks something like this:

So my question is, any idea how I could automate the assignment of the net name to the value of the component? I tried ${NET_NAME} in the value field but that obviously does not work. Any ideas?

Thanks in advance!

[Jules]

Can you try NET_NAME() ?

See List of all text variables available in nightly builds - #6 by JeffYoung

I recall having to use { } instead of ( ) but that could be me.

[JeffYoung]

NET_NAME needs a pad number. So in your case it would be ${NET_NAME(1)} (assuming the single pad in your test-point footprint is numbered “1”).

[ekoeck]

Ok, thanks, makes sense. Doesn’t work with 6.11 but I will try again once Debian 12 is out (and I can upgrade to v7).

[scandey]

I had no idea this existed and I’m incredibly excited to use it on my next board! Thank you for sharing it!

[JeffYoung]

Doesn’t work with 6.11…

Yes, this feature is new in 7.

[ekoeck]

Ok, it’s working fine with one downside: it shows the full path of the net name which is not really necessary. I tried using SHORT_NET_NAME(1) but this does not seem to work in the value field

[JeffYoung]

${SHORT_NET_NAME(pad_number)} not supported (#15095) · Issues · KiCad / KiCad...

(I’ve pushed a fix to master so it will be in the next nightly. You’ll have to wait longer for 7.0.7…)