Electra Panels

Right Click on the Main Menu to pop open the panels dialog.

That's it !

Annotate Reference Designators from a Text File

One method is to use Schematic Editor > Tools > Annotate > Back Annotate Schematics and load in a Was-Is file. The Was-Is file is simply a text file with the current designator a space (not tabs) and the new designator on each line.

C1 C4
C2 C3
C3 C2
C4 C1

The file name has a .was extension.
This will change both the schematic and the PCB designators, not just the PCB designators.
Copy / pasting from Excel to a text editor works but you will have to change all the delimiters from tabs to spaces. 

If you want to change only the PCB side then paste into the string column of the designators in the PCB List panel and re-link components by designator should work.

Source: 

Annotate Reference Designators from a text file? - Altium Discussion Forums - Eric Albach

That's it ! 

NetTies and PAD Classes

Pad Class can be used to suppress Net Tie Hole to Hole Violations.

As shown below two multilayer pads were place on top of each other to create Net Ties that can be used to connect tracks or copper on any layers.

Design > Classes > Pad Class > NetTie PADs

Design > Rules > HoleToHoleClearanceNetTies

That's it !

Electra Do File Tweaks

To clear existing routed tracks and vias, except GND and Diff Pairs.

Altium > PCB Fliter

(IsTrack or isVia) and OnSignal and not InNet('GND') and not InAnyDifferentialPair

Delete Filtered Selection

Altium > Script > Export Specctra DSN

# My Do

select all nets
unselect net GND
unprotect all wires
unprotect all vias

lock net GND
protect net GND
protect all dpairs

print {Tax via 5 (high)}

reset

tax via 5

bestsave on "tax_via_5"

autoroute

report summary "tax via 5"

# End My Do 

Electra > Altium  

Electra

Run My Do

File > Export Routes 

Tip:

Do Not Assume any Existing *.rte files are good, always Export > Routes

Altium

File > Import Specctra Route

Design Netlist > Clean All Nets

Run DRC > Review and Fix as Needed

Altium PB Filters

Istrack and OnSignal and not InAnyDifferentialPair

(Istrack or IsArc or isVia) and OnSignal and not InAnyDifferentialPair and (Keepout = 'False') and not InNetClass('PWR')

Altium

Route > Retrace Selected (Shortcut Keys UC)

Tips: 

Altium

Preferences > PCB Editor > Gloss And Retrace > Miter Ratio 3

That's it !

Tools > Import / Export Mechanical Layers

Tools > Import / Export Mechanical Layers

Includes Layer Pairs

That's it !