How to have copper fill include mounting holes

[Douglas777]

I specified the clearance for the copper fill as being about 2 or 3mm, bearing in mind that there are high voltages around the connectors (e.g., R, S, T 3-phase mains voltage and +200V DC for motor connections).
I need to maintain a similar clearance to that which is present between the 2.54mm spaced pads of the screw terminal blocks.

The problem is that Kicad uses that same large clearance around the holes
(plastic locating stub holes for the 3-way connectors and mounting holes for the 32-way DIN connector.)
The custom rule reduces it at the PCB edge to 0.5mm.
I am wondering if there is a further custom rule that can similar reduce clearance around the holes? (Or even reduce to zero.)

[Douglas777]

Thanks - that achieves the desired reduction in the number of vertices.

The perfectionist may require that the grid boundary lines are precisely either horizontal or vertical!
Surprisingly, although “Constrain outline to H, V and 45 degrees” is checked, this does not seem to be respected.
Using a large grid, I move, for example, the single upper line to a new position.
Hovering over the left and right square boxes at the end of the boundary line then shows y=-13.21 and 113.17mm at the ends

As illustrated in the following, it is furthermore possible to drag a vertex such that the boundary is clearly not horizontal

In other words, the shape constraint does not appear to be respected … which is a bug

Of course, for this application it is simpler to just redraw as a single polygon …

I was interested in the merging possibilities since I assume similar apply for the design of things such as custom-shaped footprints.
[Maybe different algorithms are used there?]

[mf_ibfeew]

I am wondering if there is a further custom rule that can similar reduce clearance around the holes? (Or even reduce to zero.)

Wondering doesn’t helps. You have to play with kicad and the rule-system for yourself, otherwise you will always only be able to reuse the rules other people made for you. Take 2…3 hours this evening, read PCB Editor | 6.0 | English | Documentation | KiCad and select some tasks you want to fulfill with custom rules. Start with easy simple rules, start with modifying some of the rule-examples.
As a last gift for today:

• draw a little “rule area” around the holes (where you want the copper). Name the rule-area “RULE_SMALL_CLEARANCE”, select layer top+bot, unselect all checkboxes
• in the board-setup → custom-rule-section add:

(version 1)

(rule “Clearance zone to board-edge”
(constraint clearance (min 1.1mm))
(condition “A.Type ==‘Zone’ && A.Name ==‘EXAMPLE_GND_ZONE’ && B.Layer ==‘Edge.Cuts’”))

(rule “Clearance_reduced_in_ruleArea”
(constraint clearance (min 0.0mm))
(condition “A.Type ==‘Zone’ && A.Name ==‘EXAMPLE_GND_ZONE’ && B.insideArea(‘RULE_SMALL_CLEARANCE’)”))

This gives you NOT 0,00mm around the holes, but the minimal value from board-setup->designrules->constraint

project to play with is attached.
merge_zones_01.zip (25.0 KB)

In other words, the shape constraint does not appear to be respected … which is a bug

I personally would be very careful if I’m not able to use a software to directly call “bug”.
You seem to expext a different behaviour from the zone-modifying algorithm (dragging mid-line-points), but disappointed expectations doesn’t qualify for “bug”. Again play with the dragging-algorithm. Are you aware that there is the 45°/H/V-hotkey (standard: Shift+space) which influences the dragging-behaviour? (sadly there is currently no display in the statusbar for the current H/V-mode during zone-modifying - this is a bug/missing feature)