Can you set the copper clearance differently?

[NO.1_POG]

Hi All~~

When do you pour copper, Could you make it the following case?

1. Copper clearance trace clearance: 0.3mm
2. Edge line clearance: 1mm?

If it doesn’t work, what do you do?

I made keepout area.

[mf_ibfeew]

When do you pour copper, Could you make it the following case?
Copper clearance trace clearance: 0.3mm
Edge line clearance: 1mm?

simple approach: use the Board setup → Design-Rules–>Constraints and set different values for:

• minimum clearance == 0.3mm
• copper to edge clearance == 1.0mm

Additionally you can override these values with the Copper-Zone-Properties → Electrical Clearance (only in the direction of greater values)

If you have more detailed requirements you can use the custom rules feature.
For more clearance zone-board-outline for instance:

#example for extra-clearance zone to Board-edge
#the zone needs a name set in the zone-properties-dialog, in this case: EXAMPLE_ZONE
(version 1)
(rule “Clearance zone to board-edge”
(constraint clearance (min 1.5mm))
(condition “A.Type ==‘Zone’ && A.Name ==‘EXAMPLE_ZONE’ && B.Layer ==‘Edge.Cuts’”))

I made keepout area.

keepout-area != copper fill zone

[NO.1_POG]

wow Thank you so much!!~~~

1. Via hole and Edge line Clearance set up : Board setup
2. Trace Clearance set up : Copper-Zone-Properties → Electrical Clearance

Thank you!!~~~