Altium Designer - Shielding footprint "component clearance" violation
You can add a very simple extruded 3D body to the footprint:

Place -> 3D Body:


(image assumes a 0.1mm thick shield 3mm above the PCB)

Then click okay and draw the outline of your shield.

And then you make sure there's no 2D keepout on any of the keepout layers, being "Keepout" and any of the applicable mechanical layers. PCB Layer Standards on this page is helpful.

It will then use the 3D "cap" you added to check whether everything fits neatly under the cap, unless you change those rules. If it's a shield that touches the board you may want to add a line to the top layer and make that a "Keepout Line". Double click the line and in the properties check "Keepout":


If you want continuous ground under the cap's edge, which is equally sensible, you can of course add areas or lines connected to the pads, which will also prevent routing, but possibly not components.

Or if you're fine routing lines under the edge over the top (I wouldn't be, not in general at least), you can add a line on a component placement layer instead just to avoid anything ending up there that the cap will cut through.



You can alternatively make an exception, but then you are free to place too high components under the shield. If you do it like above, it will warn you with an error if you try to place a 5mm capacitor under a 3mm high shield. The margin for that can be found in the Design Rules -> Manufacturing section.