I designed a PCB in Kicad 5. The I had to change my design, but this time I did it with Kicad 6. To my surprise placing an 0805 resistor footprint from standard library next to an existing one showed that the size changed! In both cases it was hand-solder pads.
I can’t find information about changing pads sizes from version to version. I realize that the libraries changed, but though it only concerned components grouping. I haven’t tried many other components, just caps and resistors.
I do not have a direct answer to your question, but I use my own footprints for hand soldering. One is a minimal 0805 footprint which I use mostly for easy soldering of 0603 chips. The other is a fatter 0805 for places where I am really planning to use an 0805. A 1206 footprint seems longer than needed for an 0805 so I do not use that.
I like to design my boards to make hand assembly as easy as possible. If you will be doing the hand soldering yourself, then use footprints that work for you.
There can be no progress without change.
Different software versions, different libraries.
If you use your own libraries, then you have the benefit of knowing what’s in it, but the disadvantage of the progress made by “the community”.
In Kicad V4 or some other older version, all solder mask cutouts for the stencils were rectangular, and this was changed to rounded corners because it is better.
Solder paste tends to stick in sharp corners, and with round corners the paste deposit is more reliable and accurate.
Sharp corners are impossible to make, there is always some rounding. (for example the laser radius)
It’s also according to IPC guidelines.
If you want to keep the footprints uniform within a project, then create a library from the existing PCB with: PCB Editor / File / Export / Footprints to Library, add that library to the project and explicitly point the links in your schematic to that library.
Solder blob size is also not an exact science. Some EDA software manufacturers even have different versions of libraries. For example relatively big pads that are easy to get reliable, and variants with smaller pads that let you put parts closer together, but which mandate the need for more precise P&P machines, and other parameters such as smaller solder balls in the solder.
With program I used before KiCad I had one 0603 footprint for resistors/capacitors/ferrite beads and never got an idea to have different ones. When I installed KiCad (4.0.7) for the first time I found that there resistor 0603 footprint is different than capacitor 0603. I specially liked resistor 0603 as it had 1mm space between pads. I thought - if I will use 0.2mm tracks and 0.2mm clearance I will be able to route 2 tracks under my resistors (my dreams come true). I even found a resistor datasheet with the footprint exactly like that KiCad’s one. But unfortunately my contract manufacturer didn’t approved that resistor footprint. They use different manufacturer resistors (with little bigger contact areas) and assuming assembly tolerances they told me that space between pads should be 0.85mm (absolute maximum they can accept is 0.9mm).
When shortly later KiCad V5 was introduced I noticed that 0603 reasistor has now 0.85 mm space under it. I didn’t checked it in V6 yet (I’m still using 5.1.12).
If you don’t want this to happen, then you need to maintain and control your own libraries, where “you” means your company or you personally depending on your situation. You might start with someone else’s library, but you need to make it your own if you want to guarantee no changes. This will be true no matter how hard one might wish it is not.
Sometimes footprints change for good reasons, like the rounded corners on solder masks mentioned above, errors that get corrected, or pads that get modified to improve assembly yield. Other times the reasons may seem obscure and arbitrary.
I do the same but use 1206 for jumping over tracks or more power or higher voltage. Except for some values < 0.1 ohm I do not use 0805 resistors. Capacitors are different; I use capacitors in 0603, 0805, 1206, and 1210.