Greyed out vias in altium
It is unclear what you refer to as &quot;greyed out&quot;, but for instance, the via on the left(GND) is not &quot;greyed out&quot;, but it simply does not have a pad/annular ring on this layer:

The dark area (which is what I'm thinking you are referring to as &quot;greyed out&quot;) is simply an area without copper.
This is consistent with the Via Stack you posted and at which jsotola's comment hints at.
One way of obtaining such vias is editing the stack manually, changing the diameter for each layer. Another option is to use the &quot;remove unused pad shapes&quot;:

To remove unused pad shapes, select Tools » Remove Unused Pad Shapes


From Altium documentantion.
Some reasons to remove unused pad shapes:
1 - Leave more copper on the desired layer (since unconnected vias do not have annular rings)
2 - Gives more space in inner layers if clearance is a concern
3 - Less copper to drill through helps lengthen drill bit life
Honestly, 90% of the reason for me to do it is the first one, but I guess it will vary depending on who you are.
Also worth noting that due to the way plating works, its not possible to remove the Via shapes on first/last (top/bottom) layers.
This seems poorly documented/discussed so take it with a grain of salt: It seems that removing unused pads increases reliability for PCBs that suffer intense thermal cycles (but apparently it also reduces reliability in other contexts).