Slice Tracks - Options

To bring up the Slicer Properties Dialog 

Select Edit > Slice Tracks > Left Click Mouse to Start Slicing then Press the Tab Key

That's it !

Release Checks

Review Schematic, BOM and Variant Parts.

Review all required electrical and mechanical design constraints.

Review return paths, look for signal traces crossing moats in GND pours.

Review all project outputs for Fabrication and Assembly.

Review Solder mask, Solder Paste and Silkscreen. Fix as needed.

Check Board Fiducials, Markings PCB and PCA numbers.

Check Position of the Database Origin.

Check Fab Dwg - Notes, Dimensions, Drill Table, Stackup and Impedance Table.

Check Assembly Dwg - Notes and Dimensions.

Check for Antennae Nets (Vias and Tracks).

Check for Components and Pads on Mechanical Layers.

Check for No-Net Copper (Vias, Track, Arc, Fills, Regions, etc. . . 

Execute Selection Filters and Check the Properties Panel for Selected Objects.

Select Pads with No Paste Enabled 

Pads - Select  Pads with NO Solder Paste

(ObjectKind = 'Pad') And (PasteMaskEnabled <> 'True') And IsSMTPin

The selected PADs may Include Thermal Paddles with Windowed Paste.

The selected PADs may Include Fiducials, Fiducials should not have Paste.

Suggested solution for Windowed Paddles and Fiducials is Paste Enabled with -100% Expansion.

Nothing should be selected after executing the PCB Filters shown below !

Tip: Zoom Out (Short Cut Keys VF) before executing each Filter.

Components - Select Components that are Not on Top and Bottom Layers

(ObjectKind = 'Component') and not OnOutside

Dots - Select Text Strings with Zero Height (Height should be > 0)

(ObjectKind = 'Text') And (AsMM(TextHeight) = 0)

NPTH - Select NPTH Pads with Plated Enabled

((HoleDiameter >= PadXSize_AllLayers ) OR (HoleDiameter >= PadYSize_AllLayers)) And (PadIsPlated = 'True')  

Pads - Select Thru-Hole Pads that have Paste In Pin 

(ObjectKind = 'Pad') and IsThruPin And (PasteMaskEnabled <> 'False') 

Pads - Select Pads with Excess Solder Paste

IsSMTPin And (PasteMaskExpansionMode = 'Manual') And (AsMM(PasteMaskExpansion) > 0)

PTH - Select ThuHole Pads with Solder Paste (Paste in Pin)

IsThruPin And (PasteMaskEnabled = 'True')

Pads - Select Pads that are Not using Rule Based Soldermask Expansion

(ObjectKind = 'Pad') And (SolderMaskExpansionMode <> 'From Rule')

Regions - Select Free Regions with Exposed Copper

(ObjectKind = 'Region') And (SolderMaskExpansionMode <> 'None') and OnOutside and Not InComponent('*')

Tracks - Select Tracks with Exposed Copper

(ObjectKind = 'Track') And (SolderMaskExpansionMode = 'Manual') And (AsMils(PasteMaskExpansion) = 0) and OnOutside

To Fix a Pads in a PCBDoc Select Components > Unlock Primitives

After executing a Filter use Find Similar and Properties Panel to make changes.

Paste Mask and Solder Mask - Examples for Pads:

Properties Panel > Select Pad Stack > Simple > Solder Shape > Rule Expansion

Properties Panel > Select Pad Stack > Simple > Paste Shape > Enabled and Manual 

Paste Mask and Solder Mask for Free Regions and Fills in PCBDoc:

Properties Panel > Select Pad Stack > Simple > Paste Shape > NOT Enabled

To Find Fills and Regions on Paste Layers

((ObjectKind = 'Region') And (Layer = 'TopPaste')) or ((ObjectKind = 'Fill') And (Layer = 'TopPaste')) or ((ObjectKind = 'Region') And (Layer = 'BottomPaste')) or ((ObjectKind = 'Fill') And (Layer = 'BottomPaste'))

Then - Select Components > Lock Primitives !

Components and Designators Filters

Components - Select All Components Except Caps and Resistors

(ObjectKind = 'Component') And (Not(Name Like 'C*')) And (Not(Name Like 'R*'))

Components - Select Parts with Designators Like R* or C*

(ObjectKind = 'Component') And (Not(Name Like 'C*')) And (Not(Name Like 'R*'))

Designators - Select Designators with Silkscreen Violations

(ObjectKind = 'Text') And (StringType = 'Designator') And (Layer = 'TopOverlay') and HasViolations

Stackup Folder - readme.txt file

Do not delete this file.

Refer to the Stackup in the Fab notes

If available a copy of an approved fabricator stackup may be placed in this folder.

That's it !

Bug - Zero Height Text

Altium Designer Version AD23.9.2 

Altium Bug Crunch #22010

Zero Height Text strings can be created and displayed in a PCB on any layer.

Note these zero height strings will NOT be generated in the Gerber outputs.

Zero Height Silkscreen Polarity Dots will not be generated in the Gerber data.

Related Points of Interest.

The zero height strings will be displayed in Draftsman

The zero height strings will be displayed in 3D PDF files.

The zero height strings will NOT be displayed in the Gerber data.

To Find and Fix all Zero Height Text Strings.

PCB Filter > (ObjectKind = 'Text') And (AsMM(TextHeight) = 0)

In the Properties Panel set the Text.Height to a value greater than zero.  

Example Silkscreen Text.Height  = 0.001mm

That's it !

Modal / Non-Modal Properties Panel

The Modal /  Non-Modal Properties Panel Option can be set in the preferences as follows.

Checking Double Click Runs Interactive Properties will disable the Modal Properties Panel.

Unchecking Double Click Runs Interactive Properties will enable the Modal Properties Panel.

Known Issues: 

While the Interactive Panel is faster and more convenient to use it can be an accident waiting to happen because double clicks followed by key presses will modify the Default Property in the Panel.

Examples:

Double Click on a Component and you may accidently end up changing the Designator.

Double Click on a Via and you may accidently end up changing the Diameter.

Double Click on a Track and you may accidently end up changing the Width.

Interactive Panel Pros:

For quickly changing the Width of Selected Tracks the Interactive Panel is convenient.

For quickly changing the Diameter of Selected Vias the Interactive Panel is convenient.

Interactive Panel Cons:

Accidental changes are easy to make.

That's It !