Polygon not connecting to Pad

Are you sure that all 4 pads are connected to proper ground? I suggest to reduce number of pads to 2 and check, if the problem still exist.

I haven't had problems with net ties connecting to poly pours, so it can work.

The "solder bridge" component type should be "Net Tie". It should be a component, not just two pads of different nets with a track drawn between them.

If you placed the track between GND and AGND, the clearance rules are likely keeping the poly pours away.

You could also try: Tools > Netlist > Updates Free Primitives From Component Pads

The whole thing (the 4 pads and the little track between them) are a component and I defined it as a Net Tie. There is no extra track connected to the pads in the PCB (other than the bridge in the middle which is part of the component). Isn't that the correct way? I tried "Update Free Primitives From Component Pads" and also re-poured. It didn't have any effect.

What clearance rule do I need? I have just the default one in place with the numbers altered. I found that if in the matrix of that clearance rule, I change the value for "Poly - SMD Pad", it doesn't affect those particular pads, and not the other GND pad in the picture either, probably because the rule also contains "Different nets only". But anyways, looking at that other GND pad, we can see how big the clearance is and how wide the relief is, and there would be space for that in my net tie, so I don't understand why it's not connecting.

All 4 pads have the correct "Name" in the component editor (the left pads both have "1" and the right pads a "2") which translate to GND, GND, AGND, AGND in the PCB (as can be seen when zooming further in), and that's all correct. I tried what you suggested anyways (only one pad on each side). The problem still exists.

A little update on this: I tried what happens when I remove the connecting track between the pads (in the component). Interestingly, then the pads connect to the polygons with relief, just as expected. But that's not a solution since the component is no longer a Net Tie now, and I cannot place that connecting track in the PCB editor either.

Try switching off the polygons (unpoured), then place a track from large GND pad to Net-Tie GND pad.

Also from large AGND pad to AGND Net-Tie.

Then try re-pour all, with "Pour over same net objects" enabled.

Ah, my net-tie footprints are just two rectangular pads which overlap slightly and that works.

Having two pads with connecting track or fill, as I think you have, doesn't work.

Don't think that gotcha is anywhere in the documentation!

I was not able to solve it. I tried unpouring and then placing tracks. That works, but still there is no connection between polygon and pad (other than the track). I tried removing the bridge track in the footprint and replacing it with a narrow pad. This doesn't solve it either. Having only two pads could maybe work, but there is no available pad geometry to make a usable solder jumper out of two pads (i.e. one that can easily be re-closed by soldering after the bridge has been cut).

My workaround for now is to connect to the polygons with tracks. I'm not that happy because unless I connect these tracks to another object, CS tends to remove them sometimes.

OK, I think you want a net-tie footprint that leaves the option of cutting the net-tie (for measuring current perhaps) and using a solder bridge repair.

My preference for that is to use two seperate footprints.

I have test points on each net which are large enough for soldering wires (current measurement) or a link (repair).

The net-tie is a seperate footprint (just two overlapping pads) which can be cut.

Overlay the net-tie and jumper if you like, with appropriate rule to ignore collision.