V7: Clearance Text on Copper

@JeffYoung in the V6: Clearance Text on Copper thread you said the large clearance around text had been fixed in V7.0.

What was the fix? Because I’m seeing the same 0.32mm clearance as originally reported in that thread, after making sure the Clearance Resolution was 0mm.

Is that right? Is there a way to reduce this further? Setting a negative clearance doesn’t help.

Font is “KiCad Font”, bold, reversed and rotated 90°. KiCad version is 7.0.2.

There is a difference between the values/pictures in the old thread and yours:

  • old thread: all clearance-numbers are shown for horizontal text. There the clearance was calculated as line-spacing+ text-clearance
  • your picture: you have rotated your text and now show the clearance from the first letter to the copper - so this is the perpendicular side of the original question. In this case the letter-spacing is taken into account.

This is only intended as explanation, I have no idea if this current situation is correct or not.

Alright, you nerd-sniped me. Here’s some MWE’s:

First a recreation of the original.

And then with the text changed to ~{gggg} and the zone refilled.

This is just done on the F.Cu layer in a standalone instance of pcbnew 7.0.2, so font is default: “KiCad Font”; width 1.5mm; height 1.5mm; thickness: 0.3mm.

Sorry, I realised that’s a pretty crappy example because you can’t set clearances to 0 without a project. So here’s a new MWE! Same as before but with a schematic (consisting of a testpoint on GND) and clearances set to 0.


@Heath_Raftery : could you attach the zipped project archive?

Apart from your distance-issue it seems like the copper-fill is shorting the text (second picture).

Good idea. Be good to make sure it’s not just me.

fill-around-text.zip (11.8 KB)

thanks for the project.

some aspects:

  • try to update to 7.0.4 the next days (if it’s available for your system). For overbar-text there was a bug with too much distance between overbar and copper. This was fixed.
  • I think the bugfixes from your linked thread are all in place, because the measured distances are smaller than in the original kicad v6-thread
  • nevertheless I think there is room for improvement - the distance text-copper is not always equally spaced. For instance if I use only small letters - than there is too much space on the top.
  • But this seems to be not an easy task - there were numerous code-additions regarding this topic.
  • it may help to use custom fonts - the clearance-calculation for such system-fonts seems much better. However, I personally discourage from that solution - it opens new possibilities for problems (different machines with different or partly not installed fonts)

Most imortant aspect (and thanks for finding this): the short from copper to “gggg” string is most probably not wanted, I have opened a gitlab issue for that: zone filling creates shortage on lower case letters (#14803) · Issues · KiCad / KiCad Source Code / kicad · GitLab

If you want the distance text-copper behaviour improved than you have to open a additional issue. With multiple text-examples in the zone (lower letters, big letters, with/without overbar).

2 Likes
  • Looking forward to it.
  • I guess that’s the bit that’s not apparent to a user. As mentioned in the original thread: how small? Under what conditions? Small is okay, but definable is better.
  • Maybe. See next point.
  • I can only imagine! Really appreciate the insight and great to hear of the effort that goes into this. But I don’t want to suggest I’m asking for more sophisticated text clearance - sounds like a never-ending time suck. Is there a win-win here where default clearance errs on the side of too tight and the user defines their preference with a rule area? Or just do away with default clearance all together and require the user set a rule area if they’re going to overlap with a zone? Text is hard. Vector-perfect clearance would be great, but I guess if I wanted vector-level integration, I’d convert it to vectors.
  • Good to know.

I’m probably overlooking some important details and use cases here. But my 2c to consider.

2 Likes

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