Zone to board edge clearance

[wxE5]

How to specify the clearance from a zone fill to the board edge?

The setting Copper Zone Properties → Electrical Properties → Clearance has no effect on the edge clearance. File → Board Setup… →Design Rules → Contraints → Copper to edge clearance does in fact allow modifying the clearance. However, this prevents any components with pads to come closer to the board edge, which is not intended:

Version: 7.0.7+1, release build

[Dwardo]

Maybe you could use a Keepout area along the zone you don´t want copper and check the “keep out copper fill” box only.

[wxE5]

That’s rather complicated, isn’t it? For an arbitrary edge? My PCBs aren’t rectangular or round. The image above was just an example from a simple test file, not the actual board. My boards have an arbitrary shape with milled cutouts (designed in a CAD program and imported as DXF).

[mf_ibfeew]

File–>Board Setup–>Design rules–>custom rules

# Beispiel für extra-clearance for all copper zones fills to Board edge.cuts
# wenn eine Zone anders als die anderen sein soll: 
#  (condition "A.Type =='Zone' && A.Name =='EXAMPLE_ZONE' "))
# for this check the ZONE musthave a name assigned (in zone properties dialog)

(version 1)
(rule "Clearance zone to board-edge"
  (constraint edge_clearance (min 1.5mm))
  (condition "A.Type =='Zone' "))

[wxE5]

Thank you. Works like a charm. I was browsing for some setting somewhere. A custom rule did the trick.