Yes, you can add a footprint to a design that way. You will also have to do an Add Connection for each net you need to connect to the rest of the circuit. I strongly recommend that you do not do this. The schematic and layout will now be out of sync. Any new changes to the schematic will wipe out the part/nets that you added manually to the layout. If you need a new component in the design, just add it in the schematic and bring the new part/nets into layout using Compare/ECO and Import ECO.
I agree with the other reply. PADS is set up to flow from the schematic to the layout.
You are correct that you need to add a component; you cannot just add a decal from the library. So to add a decal, it must be defined in a component first.
That being said, you can do make changes in Layout; sometimes that is just easier. The trick is to make the changes in the PCB, and then make the same changes in the schematic. You could then 'ECO from PCB', but you'll probably end up needing so much clean up in the schematic that it is easier to update the schematic manually. After you update the schematic, do a 'Compare PCB' in the 'PADS Layout Link' dialog box to make sure the schematic and the PCB match. Otherwise your changes will be lost when you 'ECO to PCB'.
To answer one part of your question - Yes, you need a Part. I can see how it might not make sense to a noob, especially if you come from a different layout package, but that's how PADS works...
BTW, I agree with the comments above. Adding parts/connections (unless they are legit non-ECO parts) manually is dangerous, especially if you want them to stay in place. Any update from the schematic can and/or will remove them. Unless, of course, they were also added to the schematic (which would be a backwards way of doing things - but I have done mods that way before - not by choice though).
Proper usage of the non-ECO Part would mainly be for fiducials and mounting holes that have no electrical connection. There may be a few other uses for non-ECO stuff, but not many...
You should be able to see the library and the decals in the Add Component box if things are set up correctly. Be sure you have all four of the library files in the same folder - you need them all, even if they are empty. Then add the library into the Lib List in the Library Manager in Layout (and Logic if you are using Logic for the schematic). Select the library in the Add Component dialog box then put an asterisk in the Items box and click Apply. The decals should appear in the preview window.
If you still have problems with this please submit a Service Request and we will be happy to help you.
"Am I to assume that the library must have a part definition in it?"
yes, yes, a thousand times yes
"If that is the case, is there some way to add a footprint to a layout manually, from a library that contains ONLY footprints?"
no, no, a billion times no
you cannot add footprints to the design, you must add a Part
A Part (you may see this called Part Type) is what ties the schematic symbol (CAE Decal) to the footprint (PCB Decal)
looked at another way, a Part defines which footprint and which schematic symbol is used for the part
for example: a 100 ohm 0603 resistor (part) will use a 0603 footprint (PCB Decal) and a resistor symbol (CAE Decal)
a 1K 0603 resistor uses the same footprint and resistor symbol
but a 100 ohm 0402 resistor would use a different footprint, but the same schematic symbol