Can you give us the whole project (including gerbers)?
The irregularities around the edge of the âblobâ look suspicious. Did you cover the entire mask layer with a fill zone? This might happen if you intended to create a ground plane, but accidentally assigned the zone to the mask layer, instead of a copper layer.
Dale
The second image IS the mask layer as shown in PCBNew. Which looks correct to me. In desparation, I have started deleting things from the design to see if the mask layer resolves. No luck yet.
I hesitate to to do that. This is a project for work and the design is proprietary.
have you tried some other gerber viewers?
No but using KiCad to plot the layer as a pdf file shows the same image. So the problem is in KiCad - not the viewer.
Do you have âshow filled areas in zonesâ selected in pcb_new? If not select it. If you now see the same picture than when you export to gerber then you have a zone on the mask layer. If not then something is very fishy.
I do have âshow filled areasâ on. I have deleted everything on the board. As I deleted the components the outline of the blob roughly followed the locations of the remaining components. After deleting everything I added back a single component and the problem returned (with a really small blob).
I deleted the pcb file and created a new one. After I imported the netlist the mask looked normal.
Now - How do I salvage seven full days of work?
can you share the pcb file that only has the single component on it and still shows the problem?
Also please add your kicad version information (help->about -> copy version info)
maybe check your solder mask clearance settings?
This is a pcb file with three components which shows the problem.
x.kicad_pcb (83.4 KB)
Below are the gerber and the KiCad views:
solder mask min width is set to 127mmâŚ
2 Likes
looks like it paints strokes with a rather large brush (âapertureâ in gerber parlance, perhaps)
Where is that set? I canât find it in any of the pcbnew menus.
setup -> pads and mask clearance (for version 5.0.x)
file -> board setup (for current nightly and therefore future 5.1.x)
1 Like
Thanks - that was the problem. Obviously my fault - but I think it would be helpful if all of the rule settings were in one place. It would also be good if the layers as shown on the design screen matched the ultimate Gerber files so that errors would be more immediately obvious.
They are in the nightly build 
I am not so sure about that. It should definitely only be a view option.
I am not really convinced this would get high priority as you can easily few gerbers at the end (and should check them anyways)
This would be nice though because Iâm much more likely to notice a more subtle problem when Iâm zooming around my design at high magnification, than when Iâm reviewing the Gerbers⌠I know itâs lazy but I typically just glance at the fab preview to make sure nothing terribly wrong happened.
One option is to use the 3D viewer which I think is closer to the Gerbers⌠this is how I noticed my own issue with mask clearance the other day.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.