Gerber output without solder mask on tracks

Layout
1

Hi, I want to remove solder mask from some tracks. So I used option from track properties:

image
image1577×738 74.5 KB

The geometry is in Mask layer:

image
image937×810 51.6 KB

but in gerber files not. This is from Gerber Viewer, Mask layer displayed:

image
image1007×858 10.5 KB

Is there any seeting to change for this output or is it a bug? I’m working in version 9.0.0
Thanks.

2

Do your track is wider than 0.4mm to get any part of if mask free having mask expansion -0.2mm?

Opps. I noticed that we see in your screen-shot that its width is 1.5mm.

3

Is there any seeting to change for this output ?

No, the gerber output should just reproduce the picture from the pcb viewer. If your description is correct (and nothing important missing), then this is a bug.
But I could not reproduce this behaviour with a quick simple test (used the latest v9.0.testing from yesterday).

  • try to install one of the latest testing versions and check if the behaviour remains. There were already many bugfixes submitted since v9.0.0 release,and some of these bugfixes affected also the gerber files.
  • attach the archived example (complete project, not only the board file) in this thread, so we can try to reproduce the issue with your specific project. If you want you may delete all unnecessary items from the board.
4

Ok, I installed this version kicad-9.0-testing_9.0.0.310.gf835591c8b-x86_64-lite.exe
The problem still persist.

But I noticed when I change Solder mask setting in board setting, Minimum web width to 0
the gerber output is correct. Only zero value works.

image
image864×704 181 KB

Does it make sense if the geometry is showed in PCB Editor and not in gerber files?

this is setting I’m using for gerber output

image
image1404×756 238 KB

Here is test example…
test.zip (19.5 KB)

5

good pictures, good example. Looks really like a bug, provoked by the "“solder mask minimum web width” setting.

Would be good if you open a gitlab issue (Kicad board editor–>Help–>report bug report) and attach there your example and the pictures.

Does it make sense if the geometry is showed in PCB Editor and not in gerber files?

Normally not, gerber output and pcb display should be the same.
But there is a exception. All settings in the shown “Board setup–>Board tackup–> solder Mask&Paste” are only used for postprocessing the pcb prior to the gerber generation. So these settings (mask expansion, removal of mask < minimum web width) are not reflected in the pcb editor.

6

It looks like JP fixed this 30min ago: plot mask layers: do not skip mask on track when solder mask min web is not 0 (7f1b4122) · Commits · KiCad / KiCad Source Code / kicad · GitLab

2 Likes