Creating a "cut trace" option

[analogix]

I'm working on a design with 74HCT245 buffers where a couple of the inputs (and corresponding outputs) are unused.
(Unused buffer inputs should be grounded as far as I know, but it would be nice to have an option for using them for something else if desired or needed)

So... how about I just add a solder-pad or through hole to each of the inputs' traces (this will be the default setting), and if needed, the traces can be cut (disconnecting them from GND), and on the output side I'll have similar solder-pads or through-holes.
How would I do this in the schematic?

[voltsandjolts]

Cutting can have the downside that it's hard to go back
Zero ohm resistors or solder bridge jumpers allow you to change your mind multiple times.
https://resources.altium.com/p/solder-bridge-jumper-best-practices-pcb-design
https://www.pcblibraries.com/forum/footprint-for-solderable-jumper_topic2089.html

Oh, and don't leave inputs floating, use pull-up/down resistors as appropriate.

[analogix]

Cutting can have the downside that it's hard to go back
Zero ohm resistors or solder bridge jumpers allow you to change your mind multiple times.

I agree. I was thinking the same except that this situation should be opposite:
- normal/default setting: no need to do anything
- option setting: cut, solder, jumper etc. necessary

The "option" setting would likely be used by very, very few people, hence I'd prefer not forcing them to buy additional components (zero ohm resistors or jumpers) or remember to solder a jumper-bridge.

https://resources.altium.com/p/solder-bridge-jumper-best-practices-pcb-design
https://www.pcblibraries.com/forum/footprint-for-solderable-jumper_topic2089.html

Excellent! Thank you.
I hadn't heard about bridged solder-jumpers before, but this is probably exactly what I need if I want the above terms to apply.
I suppose it might be a good idea to route the affected traces (with the bridged jumpers) physically as far away from other traces on the board as possible. That would minimize the risk of accidently cutting nearby traces.
I tried to find bridged solder jumpers in the Eagle library but all I've found so far is JUMPER-SMT_2_NC_TRACE and JUMPER-SMT_2_NC_PASTE from the SparkFun-Jumpers library. I believe it's one of the libraries that weren't included with Eagle to begin with but that I downloaded and installed separately.

Those will work, but I prefer the "half-circle" type. Are there any other libraries with bridged solder jumper pads available?
I know I could make my own, but it's been a while since I did that and would have to re-learn the whole process.

Here's a couple of screenshots of the schematic and board where I've used bridged solder jumpers for the inputs and square vias for the outputs.
This should allow soldering wires to the unused input and output pins of the chip if the needed for some rework or another project.
(come to think of it I should probably add a couple of vias to the input traces as well, for easier and sturdier attachement of wires).

Oh, and don't leave inputs floating, use pull-up/down resistors as appropriate.

I didn't see anything about unused inputs/outputs in the 74HCT245 datasheet but found someone else's design where the unused inputs were connected directly to GND while the outputs were left unconnected to anything. Is this incorrect?
On the other hand, if I do need to use a pulldown resistor I'd be getting an unbridged solder pad for free if I ever wanted to use the (currently unused) inputs for something! 

[Doctorandus_P]

Open input can be a cause of oscillation due to the high input impedance of CMOS circuits, so in general, it's advised to connect them to "something". That can be GND, Vcc or a nearby "hard" signal. Things like this are not found in the datasheets, because it is a generic property of a whole logic family. All the mayor manufacturers have separate datasheets / application notes / descriptions of the generic properties of the logic they make.

[analogix]

Open input can be a cause of oscillation due to the high input impedance of CMOS circuits, so in general, it's advised to connect them to "something". That can be GND, Vcc or a nearby "hard" signal. Things like this are not found in the datasheets, because it is a generic property of a whole logic family. All the mayor manufacturers have separate datasheets / application notes / descriptions of the generic properties of the logic they make.

Thanks for confirming.
The only application note I've found on the subject is from Texas Instruments: Implications of Slow or Floating CMOS Inputs.
Unsurprisingly I found it highly technical and just left me more confused as it appears to say that using pullup or pulldown resistors is the way to go, and that the resistor value is important, typically between 1K to 10K.
Other technical discussions, websites and so on all suggest what you've just said: just about anything except leaving them disconnected. directly to VCC, to GND or using pullup or pulldown resistors.

What are the general rules for unused outputs? So far from my searches it appears that having an output disconnected won't cause any problems, but I also read somewhere that you shouldn't connect multiple outputs together (which will be the case if I bring them both to GND).
By the way, is it possible to add a via part symbol in the schematic part of Eagle? I intend to do so with the unused 74HCT buffer outputs (for allowing a wire to easily be soldered to it if needed), and can add vias just fine in the board section, but would like to reflect this in the schematic.
There doesn't appear to be any "via" in any of Eagle's part libraries.

[Doctorandus_P]

Never tie (active) outputs of logic IC's together, it creates a short if the outputs attempt to pull the net into opposite directions, resulting in a higher current draw, IC's heating up, and possibly damaging them. Leaving outputs open is the best way here. With analog circuitry it's different. Unused opamps for example should be properly passified, and the proper way to do that is dependent  on the actual opamp. Often they are routed as  a "buffer" with the open input tied to GND, but some opamps are not unity gain stable.

For your "vias". Yes, it's good practice to plan ahead so you can more easily make modifications later to (experimental) circuits. In KiCad I use the "test point" symbol for this, but you can use any one pin connector, and then you have a THT (or SMD) pad you can use to tie some other signal to.

If you have some left over area on your PCB, you can also place some single row THT connectors next to each other. This creates a little experimentation area that you can use later for small modifications or extensions. It's not very useful for a "polished" design, but can be handy if you have some doubts about sections of your project, but still want to order a PCB for it.

[langwadt]

running the track through a through-hole pad might be easier, because then cutting is just a quick twist with a drill like on veroboard