KB: Pour polygon to connect the same net copper objects inside the outline
Created: May 07, 2024 | Updated: July 01, 2024
Altium Designer
Starting in version: 18
Up to Current
[Why] Polygon won't pour to connect the same net copper objects inside the outline
[What] There can be several factors that can prevent polygon pour from establishing connection with the same net copper objects, such as: incorrect Net Options and Polygon Fill Mode attributes, Polygon Rebuild option in Preferences, incorrect or incomplete Layer stack definition/assignment, incorrect Pour Order among multiple overlapping polygons, Electrical Clearance rule set with excessive value, Polygon Connect Style set to 'No Connect', and/or hidden Text object on the same signal layer
[How] Review each of the above, and if all else fails, start stripping the design to a simpler form (after you make a copy) to narrow down on the culprit.
Solution Details
There can be several factors that can prevent polygon pour from establishing connection with the same net copper objects, such as:- 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
- In Preferences, Polygon Rebuild option unticked
- 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
- Incorrect Pour Order among multiple overlapping polygons in Tools » Polygon Pours » Polygon Manager
- 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-to-create-a-net-tie
- Polygon Connect Style rule set to 'No Connect' for pad or via
- In View Configuration Panel, on View Options tab, under Object Visibility section , Texts objects on the same signal layer may be hidden