Copper fill clearance?

[frankie]

Hi everybody !

I’m struggling with my copper fillings : I want to add a copper zone on my back copper layer.

To me, 3 zones are not filled as they should be ; the copper zone should come closer to :

• my board outline (1)
• my pads clearance zone (2)
• my connector J1 (3)

Do you have any idea to change this please ?

Thank you very much !

[Rene_Poschl]

each zone has separate clearance and min width settings.

In open gl canvas:
Open the zone properties dialog by pressing e while over the zone outline outline. Or via the right click menu.
I don’t know how to get to this dialog in legacy canvas.

[dchisholm]

@frankie

the copper zone should come closer to :

my board outline (1) [/quote]
The “Fill” algorithm seems to treat an Edge.Cut as if it was a trace. This means it will leave a gap equal to the zone’s “Clearance” parameter between the edge and the filled zone. Reducing the “Clearance” parameter will reduce this gap. However . . . . the board fabricator will require a minimum “setback” between the board edge and any copper feature (zone, trace, pad, etc). The board-edge setback requirement is typically greater than the copper-to-copper clearance requirement in the layout. Therefore you may want to retain the wide gap at (1).

. . . my pads clearance zone (2)

@Rene_Poschl gave you the solution for this: Change the “Clearance” parameter for the Fill Zone

[quote] . . . my connector J1 (3)

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.

Dale

[Sprig]

@frankie

Do you have any idea to change this please ?

@frankie Welcome to the KiCad forums!

1. 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.

2. 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.

3. 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.

[Joan_Sparky]

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).