Altium individual clearance for polygonpour
You should create a pad class and add the pads you want to have a larger clearance to it. Go to Design -> Classes, right-click "Pad Classes" in the left-hand pane and select "Add Class". Name the class and in the "Non-Members" pane select all of the pads you want more clearance around. Use ctrl+click for multi-select. Then click the ">" arrow to add the pads to the "Members" pane:



Click "OK". Then in the design rules under clearance create a new rule, and for "Where The First Object Matches" select "Custom Query" and use "inPadClass('myPadClass')" Set your clearance, click "Apply", and then "OK": 



The new rule will only apply to the pads that you have added to "myPadClass".