Assigning multiple labels to a single net results in kicad selecting one of them. A priority list is used to make this decission:
- The lowest priority are local labels.
- Next priority is a hierarchical pin/label.
- The highest priority are all global labels. This includes both power symbols and global labels (power symbols are global labels).
If you have multiple labels of the same priority then KiCad will choose one of them. I am not aware that the behaviour is documented in this case so for us users it might as well be random.
So what does it mean for you? Well you might want to rethink your use of global labels for connecting stuff that should be connected directly to ground.
I have not seen the rest of your circuit but it seems quite dodgy that you connect a thing that seems to be a GPIO (assumed from the name of the label) directly to ground and that not directly at the pin but somewhere else. (remember a GPIO can be a output pin, you are one programming error away from trouble.)
I assume you use global labels because you are using multiple pages. I am generally of the opinion that global labels are not the best choice to go about these things as they require knowledge of the full design at every decision (there is no isolation of knowledge domains). So it might be better to switch to hierarchical pins (and therefore true hierarchical design). See Hierarchical or flat schematic design, what is best for me? (How to deal with multi page schematics?)