How to query wires that are connected to selected component in Altium Designer?
May be one of this helps:

For rules like track min with:

Open Project options -> Class Generation and enable "Generate Net Class for Components".
After you did sync this to your PCB you can define a design rule (e.g. track min with) valid for all nets which are connected to e.g. IC123. But you Design rule will get quite unmanageable as you need to define either many rules or one rule with many "OR" (... OR IC123 OR IC456 OR IC789...) AND you will run into troubles when annotating changes the IC Designator

e.g. for clearance rules:

In the schematic: add a parameter name "ClassName" value "exclude_8mm_clearance" to every IC you want the clearance rule be applied. This will add this devices to the component class "exclude_8mm_clearance" In the PCB design rules add "NOT InComponentClass('exclude_8mm_clearance')" to your design rule to avoid DRC clearance errors for this specific Items.