PCB Filters

Select all Traces on Top Layer

isWire AND onTopLayer

Select All Traces with No Net

(ObjectKind = 'Track') And OnCopper And (Net = 'No Net')

Select Floating VIAs
(ObjectKind = 'Via') And (Net = 'No Net')

Select Fills

IsFill

Select  Components by Name, i.e. Caps

Name Like 'C100'

Name Like 'C10?'

Name Like 'C*'

Select Footprint by Name

Footprint Like 'SOT65P210X110-6L'

Footprint Like 'CAPC1005*' 

Select Pin Number in a Component
HasPad('J201-1')

Find Free String Child Objects of Components
(StringType = 'Free') And (Component <> 'Free')

Select VIAs and Pads by Hole Diameter

HoleDiameter = 0.2

HoleDiameter Between 8 And 10

Select Comments Not on Silkscreen

IsComment And Not OnSilkscreen
IsComment And Not OnTopSilkscreen

Select Hidden Comments

IsComment And (Hide = 'True')

Select Top side Component Comments 

(InComponentClass('Top Side Components') AND IsText) and IsComment

Select  Bottom side Component Comments

(InComponentClass('Bottom Side Components') AND IsText) and IsComment

Select Hidden Designators

IsDesignator And (Hide = 'True')

Select Top side Component Designators 

(InComponentClass('Top Side Components') AND IsText) and IsDesignator

Select  Bottom side Component Designators  

(InComponentClass('Bottom Side Components') AND IsText) and IsDesignator

Select Designators on Bottom Overlay (Silkscreen)
(ObjectKind = 'Text') And (StringType = 'Designator') And (Layer = 'BottomOverlay')

Find Lost Polygons - PCB Filter then use PCB List Panel 

IsPolygon And OnSignal And (PolygonRemoveDeadCopper = 'True')

Find Parts with Population Parameters = DNI 
(ObjectKind = 'Part') And HasParameter('Population', 'DNI')

How to Apply Queries to Filtered Results
Additional Queries should be qualified by the use of the IsSelected keyword, in conjunction with the And operator.

How to Comment Queries {Using Brackets}

Not OnLayer('M5 - Dimensions') And IsDimension {Determine if any dimension objects in the PCB are *not* on the Mech 5 Layer.}

Select Board Outline 
(IsArc OR IsTrack) AND OnLayer('Board Outline')

Also See:
Create PCB Filters Using Find Similar

See Wiki - Altium for:

PCB - Filter Panel
Schematic Filter Panel