Problem creating fill zones and board outline

In PCBNew I can no longer fill zones. I’m not sure what changed. This worked fine in version 4. I thought I had it working once already in version 5.0.1, but I’m not sure. I think the problem has something to do with the polygon drawn on my Edge Cuts layer, because launching the 3D viewer generates the error “Unsupported DRAWSEGMENT type Polygon”, and KiCad complains it is unable to determine the board outline.

I can demonstrate this by creating a really simple design with one resistor, one capacitor, VCC, GND, and PWR_FLAGs. I assigned the resistor and capacitor to SMD footprints. Then I launched PCBnew and with default design rules I set the layer to Edge Cuts and drew the board outline with the Graphic Polygon tool, leaving plenty of space around the components. Then on the F.Cu layer I routed a trace between one end of the resistor and capacitor and I connected the opposite ends of each through vias on B.Cu so I could do something useful with a ground plane. Now I selected the B.Cu layer and create a rectangular GND zone around the components but well within the board edge. Then I select the zone boundary and use right mouse to select Fill, but the zone doesn’t fill and I get no feedback other than a dialog that gets displayed and dismissed so fast that it is impossible to read. Launching the 3D viewer generates the error “Unsupported DRAWSEGMENT type Polygon” and KiCad complains it could not determine the board outline. The 3D viewer also shows that B.Cu did not fill with copper.

Even if I omit the creation of a ground plane in my designs, uploading a design to OSHPark suggests there is something wrong with the result, because the Top and Bottom views are completely blank, though all of the individual layers appear to be correct and the web page does not complain of any errors. The web page instructions state that if Top or Bottom are “all white”, then there is something wrong with the design and one should check for “gaps”. I’m not sure if all black for Top and Bottom represents the same type of problem, but I suspect it does.

I’ve tried all sorts of variations on this, including several variations of design rules and even uninstalling KiCad 5.0.1 and installing version 5.0.0. No one else seems to have reported a similar problem in the forums.

Solution: don’t draw polygons on Edge.Cuts. Use segments (lines).

Edit: Edge Cuts Outline Versus Color Filled


And the bug report for this:


That did the trick. Thank you.

The bug has been marked as “fix commited” lets see with tomorrows nightly what that means.

commit 1858b7dca7a6b38d52a6360783d7c4cd02e33c38 (HEAD -> master, origin/master, origin/HEAD)
Author: Seth Hillbrand
Date: Sat Dec 1 21:41:17 2018 -0700

pcbnew: Allow closed polygons as board edges

Like circles, polygons are self-closed elements that define an outline.
This allows them to be used as such for board outlines and cutouts.

Fixes: lp:1795563

I am kind of curious what that means.


commit d3a67e255df7a0048ef5f201836af36ac456d4c9
Author: Seth Hillbrand
Date: Mon Dec 10 06:08:03 2018 -0800

pcbnew: Polygon tool on EdgeCuts adds polylines

Edge cuts are more easily edited when they are polylines not polygons
and this keeps the files backwards compatible with v5.0.x.

This is my fault; I noticed that edges made with new polygons weren’t compatible with 5.0 and gave notice. Now the polygon tool can be used but the result is a polygonal bunch of segments.

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