Thanks, that was most helpful - I have analyzed that, and add it to the bug report.
Turns out the PcbNew does have a bug where
Trace-FillPolyline-Connect is OK
Trace-Pad Connect is OK
but PAD-FillPolyline Connect is not using the PAD Outline, instead it uses the Pad-Centre.
As a result, there are many false-connect errors.
Have PAD-FillPolyline Connect, changed to properly use the PAD outline.
LHS is your close to your default rules, and a trace added and tuned until it just connects, via Trace-FillPolyline-Connect Code.
RHS is rules made smaller on Width & Clearance, so that two spokes generate, but still Connect fails.
If I make even smaller again, ie lower width, and lower clearance, then when the FillPolyline CentreLine includes the PAD centre, the PAD-FillPolyline Connect now passes.
FillPolyline CentreLine is not visible, but if you switch to fill outlines mode, you can estimate it.
eg in the case here, reducing to
A clearance of 0.35mm and FillLineWidth of 0.15 just fails Pad-Centre check
A clearance of 0.35mm and FillLineWidth of 0.125 just passes Pad-Centre check
In this last case, DRC gives no errors and no not-Connects.
Smaller FillLineWidths used to be avoided to keep Gerber sizes from ballooning, but KiCad has option for Polygon fill, which drops file size.
Also FillLineWidth defines the sliver-size in Gerber, so should not go too low (> 5 mil?)
Checking on this design for fill modes vs file size @ 0.125mm LineWidth
Segment-fill -> 502k
Polygon Fill -> 108k
So the cost for a segment fill is not too bad.
Personally, I’m wary of Polygon fill, as that uses / assumes a smarter Gerber post process, and we had a file badly broken a couple of years back, when the PCB house edited it using CAM 350, and the saved file changed the Fill-Orders. They gave us new boards, but it did cause a delay.
GerbView seems fine with both modes.