There is a second (and possibly third) factor to consider here. The Fill algorithm has a “Minimum segment width” requirement. After allowing for the required “Clearance” around the connector pads, the algorithm will NOT fill an area that is narrower than the “Minimum width”.
The specific area pointed by your arrow “3” meets the criteria for “clearance plus minimum width”, but it is not filled because the fill will be an isolated island, without electrical connectivity to any other copper in the same net.
Draw the zone outline outside the edge cuts layer. This can be quite a bit outside the edge cuts layer and still be fine in my experience.
There is an oddball setting under “Dimensions” for “Pads Mask Clearance”. My recommendation is to set this to the same value as the “solder mask to copper” clearance settings your Fab house minimums has for the trace specifications.
If the above settings don’t help on this issue, then you are going to need more board real-estate.
These are complex questions, and not so simple answers. But, I do hope this gets you going in the right direction.
Don’t forget that the setback of the filled zone vs edge.cuts does work the same as it does for tracks - it measures to the EDGE of the line width of the edge.cuts line drawn - same as it does for tracks.
So if you want a larger gap to the edge of the board vs. what you have towards other parts of your design (tracks, vias, etc) just modify the edge.cuts line width - thicker will cause a larger gap towards the edge of the board, which is defined as the CENTER of the edge.cuts line(s).