# In EAGLE, why is the ground pour not connected to these SMD pads?

There are some SMD pads in my schematic that are connected to ground, but do not appear as connected on the board. Any help on how to solve this?

This happens for all pads except 12, which is also weirdly connected

• Schematic is needed. – Leon Heller Jul 15 '18 at 15:14
• Something to do with clearances, would be my guess. – Hearth Jul 15 '18 at 15:16
• Felthry is correct: Clearance from neighboring pads is too big. Look at the "circle" near pads 5, 15 and 14 - the fill cannot reach the pads. – Turbo J Jul 15 '18 at 15:34

The isolate setting tells eagle how close the pour is allowed to get to any item not on the net. Additionally this distance is affected by DRC clearance rules, net class clearance rules, and isolate settings of other polygons.
The width setting specifies the width of the lines used to build the polygon (the fill is actually internally a series of parallel lines).
When you have narrow packages, you often find that the polygon cannot reach the pins because in doing so it would violate its clearance requirements. To solve you either need to change your settings (e.g. reduce isolate or width), or simply manually route the connections.
To manually route you only need to use the route command to draw a short trace out from the pin - far enough to meet the polygon. The trace doesn't have to connect to another pin, it will connect to the polygon when you run ratsnest.