Good morning @JonnyDex, from the first pic you show (last tab in face operation) you do not have an lead in but you do have a lead out, which is one of the potential problems I mentioned. You have a 0.1125” lead out. I am only seeing vertical in that pic. Usually there is a horizontal and vertical setting. It may be that facing does not have a lead out (I’ll get to my theory later).
FYI if you hover over almost all of the settings in the CAM there is a handy pop-up with a diagram and/or description. For instance, if someone had no idea what “keep tool down” does, hover over the check box and they get a description.
Next pic. Since you are doing facing operation, it does not have the containment properties I mention that would allow you to constrain it to the box selection. Facing needs to be able to get at the part from outside the selection so it can take off the entire face. Which is why it doesn’t have a drop down to constrain it in that tab because the facing operation starts from outside the part and ends past the part.
To get facing to behave the way you want, you may need to lie to your program about bit diameter. I personally am not a fan of lying to CAM or ignoring errors F360 throws…while it will work, it may have unexpected outcomes and devilishly tough troubleshooting to figure out why whatever happened occurred.
The part I am missing that may make facing work for you without picking a tool size smaller than it is (a valid choice that will work and may have unintended consequences), I need to see the second to last tab, the one that looks like a tank filled with water. IIRC there is a pass extension setting that tells it how far to go past the edge of the part so you. Typically values are >>1/2 diameter to 1x diameter to ensure there are hesitations start / stop swirls on the edge of a part…drive it at speed past the edge before switching direction to lift the bit.
While it seems like a good choice, I find facing to be a challenging path for facing the spoilboard. I use parallel instead. I believe it’s a 3d path, but given there are only two top level choices—2d or 3d—don’t rely on rum fueled beach memory 
For parallel, you can constrain the bit in the second tab (your 2d pic) you will have a drop down with three choices: inside, bit center, and outside. Additionally, there is an offset box that takes a distance value. I usually use center and 1/8 bit diameter offset. That will push 3/8 of the bit past the edge while keeping it within the boundary and not generate 1F errors.
Other operations are 2d or 3d pocketing. They are essentially the same with 3d being smarter about figuring out what pockets you want to cut and 2d needing to be explicitly told. In this case, 2d is where I would start since there aren’t any pockets in your model and 3d will give an empty tool path unless you give it a bounding box and depth to cut…which is essentially what 2d requires to know what to do (even if this was a real pocket)
Hopefully this helps. Sorry I can’t send pix to show my specific settings.
). Finally, the second tab boundary can either cause a problem or help constrain the bit so you don’t get errors. There are three choices in the drop down for creating boundaries, bit inside, center in boundary, and outside boundary. Additionally, you can set a +/- offset to push it further both ways.
