How and when should I split a schematic component into multiple parts
A schematic should read like a book.

E.g. (In English) The convention is that we expect books to read front to back left to right. 

A schematic is the same, you want people to be able to read it and in doing that they expect certain conventions.

As a result I will use multiple parts whenever I can (within reason):


The part has logical seperable functional blocks. E.g. FPGA banks, power and function, multiple identical functions (e.g. logic blocks).
When there are too many pins, e.g. multiple power &amp; ground banks.
When doing so will reduce clutter


I would avoid it when the blocks are more 'fuzzy' e.g. Microcontroller non-dedicated IO pins as the function is defined later not by the manufacturer.

I would also avoid it when it gains nothing, e.g. a Dual Red/Green LED. It makes it more readable if there is just one part as with two they could get separated in the schematic reducing readability.

Remember the schematic symbol need look nothing like the PCB footprint, indeed this should (usually) be avoided as it often makes the schematic much more difficult to read with wires crossing everywhere.

I never put internally unconnected, unused pins in the schematic unless they have some phantom function (e.g. a pin which must float)

To use your switch chip as an example, I'd make at least 10 'parts'.  One for control signals, 8 identical switch ports and a power/ground part.  Organise the switch ports so that the pins look neat in the schematic WRT the signal that go to the magjack or whatever you are using.

Another trick is to combine multiple power pins of the same voltage and function into a single 'stack' of power pins. That way a single schematic connection make all power connections with far less risk of error and less clutter.