Hey Dan,
It’s not that complicated: On most computers, it is Ctrl-A (select all), Ctrl-X (cut), Ctrl-C (copy), and finally Ctrl-V (paste).
EDIT: Sorry, I forgot that maybe not everybody has a keyboard and a mouse connected to the Onefinity Controller, or runs the Onefinity Controller User Interface from a remote computer (which would have the additional advantage that you can see the CAMotics 3D toolpath simulation and can also easily make screenshots of the Onefinity Controller User Interface), but instead most users are probably used to work with this ugly stupid on-screen keyboard on the touch display (which on top of being an on-screen keyboard, is missing important system keys 
). Of course, such a distasteful thing can discourage users from doing anything at all. But, you don’t forcibly need to add a keyboard and a mouse, the on-screen keyboard will also do it.
Of course, instead of clicking into the ‘tool change’ field of SETTINGS page, then typing Ctrl-A (select all), Ctrl-X (wipe it out), going to the new browser tab that you previously opened on Onefinity Controller’s chromium window or on your remote computer, where you opened the page with the example, marking the example, typing Ctrl-C (copy to clipboard), and then back on the Onefinity SETTINGS page in the first browser tab, pasting it with Ctrl-V (paste clipboard content), of course, instead of doing this, you could very well, as you suggested, simply look which lines perhaps are already there (as shown below), and then just add the additional ones from the example. This should even go with the on-screen keyboard 
You actually thought more practically here than I did in my joke above 
Making the ‘tool change’ routine usable
For example, if the content of your ‘tool change’ field on your SETTINGS page already contains the following (it usually should, as of up to version 1.0.9):
(Runs on M6, tool change)
M70
G21
S0
M0 M6 (MSG, Change tool and attach probe)
F100
(probe to minimum z soft limit, which is -10)
G38.2 Z-10.0
G92 Z15.4
g0 Z30
M0 (MSG, Remove probe, start spindle)
M72
then what Razi Ullah’s excellent example would change is just the following (add the text in bold letters and press “Save” on the flyout menu):
(Runs on M6, tool change)
M70
G21
S0
G28
M0 M6 (MSG, Change tool and tighten collet)
G0 X0 Y0
M0 (MSG, attach probe)
F100
G91 ; (added by Aiph5u, this was missing!)
G38.2 Z-10.0
G92 Z15.4
g0 Z30
M0 (MSG, Remove probe, start spindle)
M72
What will this little change do? Much!
Instead of being stuck over your workpiece at tool change, with too little room to be able to change the bit, the added G28 command will move the router to the machine origin, which is at home position, and ask you to change the bit THERE. Isn’t that comfortable? Plenty of room to change the bit, and no need to lean over the machine. Then, after you have confirmed that you are done with changing the bit, the G0 X0 Y0 command will move the router from the machine origin to the part origin (also called workpiece zero), which means the position where you probed your workpiece at the beginning, and allow you to probe Z again. Probing Z is necessary after every tool change, since usually the bits have different lengths, so this is to make the machine know the new tool length. And after you’re done with this, the machine will restore all settings and positions with the M72 command that it previously saved with the M70 command at the start (including your possibly chosen imperial measurements mode ), and voilà, the machine resumes the program and goes on with the next part with the new bit. A beautiful tool change within the program, isn’t it?
Note that this example assumes you have your workpiece zero on top of the workpiece and that you probe the top of the workpiece. Even as often there may be the case that instead you defined a 3D model with the workpiece zero on the bottom of the workpiece, which means, as you surely know, this has to be Z-probed directly on the machine bed. The Onefinity Touch Probe is used upside down in those cases. In this case you can still use nearly the same ‘tool change’ example, you would simply remove the line “G0 X0 Y0” (or better just make it temporarily inactive by prepending a semicolon ( ; ) at the beginning of the line), and the Z probing will then simply be offered at home position too, where you already changed the bit.
One thing that you could change too, is to increase the “-10” value on the G38.2 (Probe) command to a higher negative value.
This value does nothing more than to tell the machine for how much Z travel it should move downwards in order to find the touch probe before aborting. By increasing this value you can get plenty of reserve to avoid the annoying “Probe not found” error, but dependent on at which height the workpiece zero of your g-code program is, you will have to select the value that accomodates your needs.
Finally, what you can still adjust later, after you’ve tested this example, is from where you want the Z to start probing, perhaps from a lower position. If you know e.g. that your workpieces are usually rather low in height and how long your longest bit in the program will be, you can add an additional command for moving Z to a lower position prior to start probing. You can get help for this later here in the forum.
References
- How to understand and to use the content of the ‘tool-change’ field of the SETTINGS page, is to be found here ←.
EDIT: There is an updated example of the ‘tool-change’ routine in the newer posting below