My suggestion,
Check all your library parts used in the design in the library editor,
check that none of them have extraneous bits spread out away from the main
body of the part. In the library viewer window the part should roughly come
in filling the screen (either X or Y) with all layers turned on so you can
see anything on any layer. If it comes in smaller, then there is probably a
primitive spread out away from the main body of the part. Then update the
PCB parts from the library once you have confirmed your library parts are
alright. I suspect that you have gotten some primitives from a land
pattern/footprint accidently moved out to the extremes of the database. If
you get it fixed, make sure that all your land patterns have their
primitives locked so that they cannot be moved separate from the whole land
pattern again. That's my best guess at what may be going on.
To try and just remove the problem, the selection trick that should work
is actually. Turn on all used layers. Select All, then Deselect Inside
mousing just around your board outline, then Shift-Delete. The details of
this operation are: This selects everything regardless of it's location.
Then you deselect anything within the board outline. Then delete the still
selected items.
The key operation is the Deselect anything bounded by the board outline.
If it is even a segment of a land pattern that was moved outside the board
outline, that item will not be deselected by bounding the board outline.
Then when you Shift Delete, you will remove that offending item with
remnants out in the extremes because it was not deselected by the bounding
box only around the PCB outline. If this seems to work then run the Update
PCB from your schematic again, it will probably add back components that you
did delete fixing the problem. Finally run your DRC to see that everything
is still as per the rules and connectivity.
By your original comments, the only way that soldermask portions of a
part land pattern can move away from the pads is when they are added into
the land pattern as a separate primitive. Otherwise most of the normal
soldermask detail is calculated from the pads. Since you say there are no
pads in that area, then the culprit(s) must be from land patterns that have
separate soldermask primitives (fills, traces, polygons on the soldermask
layers) within the land pattern. Does that help you zero in on the culrpit
parts?