If you can't avoid what you have done, at least add thermals to the GND via, in the other layer(s) where it connects to the GND plane. This way:
1) Thermal conductance of that GND via is reduced, which makes soldering easier
2) Imbalance between the thermal conductances of the two pads is decreased (i.e., they are more close to each other in the amount of heat flow required), so that the risk of tombstoning is decreased in production.
Use as small vias as possible. 0.4mm is really pushing it. With 0.3mm, you have some chances - solder wicking effect is reduced (and the thermal resistance is higher). With 0.25mm, I'm typically having success in via-in-pad, but still, I only do it in the large pads of power devices.
If you look for an actual hard design rule, then the answer is simple: no, you can't do it - or only if you use 0.1mm laser micro vias - they have sufficiently low thermal conductance and no solder wicking occurring. If you can't afford HDI fab, 0.2mm drill is very likely to succeed (given minimal via diameter on the other layers, and sufficient thermal reliefs connecting to planes.)
Also note while others have gave you "go ahead" for hand assembly, these kind of direct vias to a large ground fill can be pain-in-the-ass to hand-solder as well! The only difference is, you can't avoid doing "quality control" while you solder, and just end up using more time and curse words, but it won't be a showstopper like in mass production.