2
\$\begingroup\$

I had a footprint for a component in Kicad 5. Then i updated to Kicad 7 and I am getting this error:

Error: Drill out of range (Board setup constraints min width 0,3mm; actual 0,2mm)

enter image description here

This worked find in Kicad 5 though. I don't know if it is related, but for clarity I will mention this here.

I am getting tons of warning on footprints not matching the library. This is after updating from Kicad 5 to Kicad 7.

enter image description here

This happens for pretty much all my footprints, but as the footprints still show on the pcb layout, I chooose to ignore these.

Finally, there is another set of error related to the one in the question. This is Thermal relief connection to zone incomplete (board setup constraints fill strategy min spoke count 2; actual 1)

enter image description here

I don't know if this error is directly related to the error in question, this is why I am also including this. Maybe this needs a different question, or maybe not.

I am getting this error on the same IC that I am talking about on the first error. However, I also get this (second) error on two more components (one capacitor, one transistor).

\$\endgroup\$

1 Answer 1

7
\$\begingroup\$

The "Drill out of range" error that you're getting means that your board setup says that the minimum allowed drill diameter is 0.3 mm, but the holes in the footprint have a drill diameter of 0.2 mm. If your fab house can do 0.2 mm drills (and you're willing to pay the premium for that if there's an upcharge), change the minimum drill diameter in the board setup.

The footprints not matching the library are just because of some library changes between version 5 and version 7; this is just letting you know that the footprints in the board cache (which are the ones from the kicad 5 libraries) aren't the same as the ones in the library now. This error is more helpful if, for instance, you make a modification to a library footprint to fix a mistake, and forget to update the footprint on the board. You shouldn't see this error on boards that aren't imported from kicad 5.

The "thermal relief connection incomplete" means that the settings currently say that all pads connected to zones with thermal reliefs should have at least two thermal spokes (to ensure a good ground connection; you can change the minimum to be 3 or 1 or even 4 if you want), and this pad has only one. If one thermal spoke is enough for this pad, you can safely ignore the error. If not, you should adjust things around the pad to give it room to fill a second spoke.

\$\endgroup\$
1
  • \$\begingroup\$ Thank you so much. Even though it turned out to be many errors in one question, you helped me. \$\endgroup\$ Aug 27, 2023 at 11:01

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.