Set all tracks and vias to net class widths in 5.1.9

In the previous version, there was a button to set all the tracks and vias to their net class values. There was also a button to join all segments in a trace or something like that. They seem to have disappeared in 5.1.9. How can I do these functions now?

Bob

Pcbnew / Edit / Edit Track & Via Properties

and
Pcbnew / Edit / Cleanup Tracks and Via’s

1 Like

Thanks Paul,

OH duh! I see what I did wrong. I wasn’t clicking on “Set to Net Class Values”. I guess I thought that was a sticky button and just forgot about it.

Now I get “Some items failed DRC and were not modified.” How do I find out which items failed? If I run DRC, all I get are a few courtyard errors, which are OK in this case.

Bob

There is a bit of ambiguity of what KiCad should do if you change the track width to the netclass value and that result would cause DRC errors.

I’m almost certain that “old” behavior was to assume the engineer knows best and thus create DRC violations because the clearances are not met.

Apparently this behavior has changed and KiCad now refuses to change the track width if this results DRC violations. The result is that tracks are left thinner then they should be. Which is also not ideal.

My preference is that KiCad would just do what I tell it to, and thus create DRC violations for clearances that are too narrow. These have to be fixed later of course, but at least DRC shows where the problems are.

It would be nice if KiCad had a way to highlight or select track segments that are below a certain width, or narrower then their net class. I am not aware of such a feature though.


But there is a “dumber” function to set all track segments to their netclass width, regardless of whether this creates DRC violations.

  1. Drag a box around the PCB, to select everything.
  2. Right click, and from the popup menu: Select / Filter Selection.
  3. Exclude everything except Tracks and vias: image
  4. After [OK], press e to edit the selection.
  5. In the Track and Via Properties, select Use net class sizes & click [OK]

Note:
This can create lots of DRC violations and this can take a long time to fix, so be wise if you actually want to do this. Making a backup of your project before you do things like this is also a good idea.

1 Like

Thanks again paul! I’ve already copied the project to the next version for this effort. This at least should let me see the DRC violations. I only realized there was a problem when I got the boards in and I just happened to see a wrong shape in the ground plane for a couple of back-side vias connected as a jumper. I had missed at least those two vias when I was checking the sizes, so I want to make sure they’re all correct. Fortunately, the current is low enough that I don’t think it’ll be a problem, regardless. But, this board has about 340 components, and if I have to make a next version, I don’t want to overlook track and via size errors again. Fortunately, this is just hobby stuff, though.

Bob

Yet another option: Pcbnew / File / Board Setup / Design Rules

This has settings for Minimum track width Minimum via drill and some more settings for other features.

Any of those features which are below the settings in this dialog will be flagged as errors the next time you run DRC.

1 Like

I had something odd happen when I put the box around the whole board. It flagged one via as an error, but it gave the wrong cause. It said that it was too close to two other vias, when it was actually too close to the pad of an LDO it and a cap on the bottom side were connected to. Should I report that? OTOH, it’s on Version 5.1.9

Bob

Upgrade to 5.1.10 before you report.
5.1.10 fixed a lot of bugs in 5.1.9.
www.kicad.org

1 Like

OK, thanks! Will do.

This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.