KB: Pour polygon to connect the same net copper objects inside the outline

Solution Details

There can be several factors that can prevent polygon pour from establishing connection with the same net copper objects, such as:

1. With the Polygon Pour selected, in Properties panel, under Propoerties section
   • Net Options not set to 'Pour Over All Same Net Objects'
   • Polygon Fill Mode set to None, Hatched with sub-optimal Track Width or Grid Size, or Solid with a large Arc Approx. value
2. In Preferences, Polygon Rebuild option unticked
3. Incorrect or incomplete Layer Stack definition (Design » Layer Stack Manager and from the drop-down, make sure there are only intended stackup defined with no duplication) and its assignment (View » Board Planning Mode or keyboard shortcut '1', double click in the green board region and select the stackup just defined)  Once setup, Tools » Polygon Pour » Repour All
4. Incorrect Pour Order among multiple overlapping polygons in Tools » Polygon Pours » Polygon Manager
5. Electrical Clearance rule set with excessive value
   • If there is a Net Tie component involved, Region connecting the two pads inside the footprint is treated to be in a different net, from which a polygon is recessed.  See also: https://www.altium.com/documentation/knowledge-base/altium-designer/short-two-different-nets-intentionally
6. Polygon Connect Style rule set to 'No Connect' for pad or via
7. In View Configuration Panel, on View Options tab, under Object Visibility section , Texts objects on the same signal layer may be hidden

If all else fails, make a copy of pcbdoc and start stripping objects and rules down to a simple form until the Polygon Pour establish a connection to the target copper object, so as to narrow down on the culprit.