Netlabels vs Ports

[Pack34]

What's the proper usage here?

Are ports for when using hierarchical design and net labels for more simple and flattened designs?

[julianhigginson]

you can do different things with them depending on how you set up the connectivity for the project.

originally ports were just a stylistic thing to visually differentiate things like power rails and references from other kinds of nets.

[tautech]

What's the proper usage here?

Are ports for when using hierarchical design and net labels for more simple and flattened designs?

That's how I use them.

Net labels are useful for power nets when you want a schematic to maintain some sort of signal flow (easy to follow) and then just place power net labels where and when you need to supply a part of the circuit or a device.
Makes for a much tidier and easier to follow schematic. 

In the Net management dialogue assign the appropriate power net label to a power trace and Altium just sorts out the connectivity in the PCB rats nest.
Use labels like VDD, V5V+, Gnd etc to make things easy to follow.

Without PCB overlays you can with insert Text assign some text to a copper layer of an appropriate size and thickness of the letters indicating the net label too. Handy for home etching where you're not likely to use an overlay.

[ajawamnet]

I typically use power objects for power distro across sheets in a project. I use netlabels local to the sheet, tho I usually make sure they are unique. I use ports for sheet to sheet connections since you can show which sheet it goes to using Report - Port Cross Ref - add to project; note that you must compile first, lest the menu option will be greyed out.

See attached...

[ajb]

Using net labels to establish connectivity is something that should be done sparingly.  Relying on it too much makes reading the schematic a time consuming game of connect the dots. 

In a design where you have signals jumping from sheet to sheet, using ports and sheet symbols allows you to establish (and show) high level connections between schematic blocks in top level sheets with implementations of those blocks compartmentalized into subsheets.  Essentially, you wind up with a block diagram where each block is a schematic diagram of a relevant section and where consistency between the graphical representation of the system and its connectivity is enforced by the compiler.  Harnesses and buses can be connected across sheets via ports, which helps simplify connectivity and streamlines schematics.  This strategy doesn't work for all designs, of course, but it's nice when it does.