Any way to find PCB info? (via size and number)

I sent a file to the fab and they’re looking to charge me extra for vias smaller than a certain size. The original design had these vias but I changed them globally and cannot find any vias of that size. Is there any way to list such things as via count and size and similar info in PCBnew?

One simple thing you can do is Pcbnew / Inspect / Design Rules Checker and then enter some value for the minimum via diameter and run the DRC.

I just discovered though that if you put n a “Minimum via size” that is bigger then your DRC rules, then this check aborts prematurely in KiCad V5.1.10. This also checks for the via size itself, and not for the drill size.

I had a look at: Pcbnew / File / Board Setup / Design Rules / Net Classes but those are not enforced during DRC.

The most reliable information is to generate a set of Gerber files, drill files and drill map file.

The drill files list all coordinates of all drills and it’s a readable text file. The drill map file is a graphical representation of the drill files and it shows the location of the various drills with small markers such as squares, crosses and asterexies.

I tried uploading example of a drill map file in .svg format but this forum does not like it, so here a screenshot of such a file as shown by Inksckape.

mumar_base_stm32-PTH-drl_map

1 Like

In 5.99 you can use “show board statistics”, under the inspect menu.
image

image

2 Likes

Script: Link
works for kicad 5.1
List the via

Change the path of the pcb file and run it using python3

If you want it in csv file, let me know

1 Like

One simple thing you can do is Pcbnew / Inspect / Design Rules Checker and then enter some value for the minimum via diameter and run the DRC.

This worked. Checking the drill file would not have worked since the hole size isn’t actually the problem. JLCPCB has a minimum hole of 0.2mm and a via pad of 0.4mm which is what I made the last iteration of this PCB to. I got an extra charge for the vias that I just paid and went with. They don’t tell you up front that 0.45mm via pads avoid the charge, and 0.2mm drill is fine. I swapped the netclass via size and went to Edit / Edit track and via properties / Set to net class values And it looked like that set them all.

Apparently it did not set any vias that had a pad clearance issue. I didn’t see any warnings and it’s hard to notice the small difference in size. Once I did the above, it pointed out all of the vias that were below minimum size and when I set them, it complained about pad clearance.