Altium: Design rule for single object in PCB
I needed to set rules priorities.

In the PCB Rules and Constraints Editor, I selected the bottom most group selecting the rules I want pro prioritize, named Polygon Connect Style, shown below.



Then I click Priorities... button on the bottom right, which brings up the Edit Rule Priorities dialog. Here you can change the priority of the rules. 

Query for single object

The query Name = '5V_Dissipator' was the only one that worked, from the three queries mentioned in the question. I believe you can use any query of the type PropertyName = 'propertyValue' to target any individual object. 

Wildcards in queries

Queries support wildcards if you use the Like operator. For example, Name Like '*_Dissipator' can be used to target all objects whose name ends in _Dissipator.

Testing queries

By far the best method to test the query you're creating is the PCB Filter Panel, shown bellow. It will dynamically show you what you're targeting.