That is a possible solution: define a keep-out zone surrounding the trace from your power pin to the bypass capacitor. The zone’s “Properties” can be defined to exclude ONLY the copper pour, while permitting pads and traces.
That statement is true as far as it goes, but there’s more to it.
The zone’s “Properties” allow you to define several types of default connections from the zone to copper features of the zone’s net.
“Solid” - this causes the fill to completely cover the copper feature - no gaps.
“Thermal Relief” - creates a gap between the zone and ALL pads touching the zone. The width of the gap is set by the “Antipad Clearance” parameter in the zone’s Properties, and the connecting spokes have a width defined by “Spoke Width”.
“THT Thermal” - this creates thermal relief gaps (as above) between the zone and Through-Hole Pads ONLY. The SMD pads have a “Solid” connection to the zone. (Probably based on the assumption that SMD components will be reflow soldered, where thermal relief isn’t necessary, while thru-hole components will be hand soldered.)
“None” - All pads, even pads in the zone’s net, are isolated from the zone by the “Antipad Clearance” value. Traces, however, are covered by the fill.
Here’s where a little more information makes things interesting.
The parameters related to connections between pads and zones can be set on a pad-by-pad basis.
The individual pad parameters can be set when the footprint is created, or after the footprint has been placed on a board. The pad parameters over-ride the zone defaults.
So that suggests a solution to the problem described by @gremlin. Recall, he has a power pin connected to a bypass capacitor, and both pads are enclosed by a zone connected to the power net. He wants to fill the zone, but leave the trace from the power pin to the capacitor pad unconnected from the zone. Here’s the plan:
Make sure the capacitor pad is physically close to the power pin. (If they aren’t, it’s probably not worth worrying about the copper fill flooding over the connecting trace.)
Edit the power pin’s “Properties”. Set the Zone Connection type to “None”, and make the “Thermal relief gap” value equal to half the distance to the bypass capacitor’s pad. (There’s a more exact formula for the “Thermal relief gap” value, but for now just trust me.)
Edit the “Properties” of the bypass capacitor’s pad. Set its type to “Thermal Relief”, and make the “Thermal relief gap” value equal to half the distance to the power pin’s pad.
Run a trace between the power pin and the bypass capacitor by the most direct route.
Fill the zone.
Did it work?