Frist very important question have you tried to run this code on the machine? Your G68.2 has the 180 that is all you need for the rotated plane to work if the machine has been setup correctly. If the part is symmetrical you may or may or see a difference in code posting the Zero position with a C0 plane or a C180 plane. What I will do to test that the post is outputting correctly is copy my C0 plane and C180 plane and shift them 1.000 in X and Y. Then just change the T and C planes to them and repost the code. If the values change then the post is respecting the correct G68.2. The biggest thing with G68.2 is are you using one base point to control all of your G68.2 outputs or are you using shifted G68.2 positions where your using reference features or other things? I for years programmed G68.2 from one point because most machines couldn’t handle the complex shifting, but as the builders have done a better job of setting up the machines I have done more shifted G68.2 programming. The code output changes drastically when the T-C plane are feature based from the part verses one point. The beauty of using mapped G68.2 is a setup person or operator can see code from that Zero point even though your G54 workoffset is the same for 50 features on your part. I have had well over a 100 different planes on one part in the past and all the code came from that one point. With using mapped 68.2 I can still have the same amount of planes, but the code zero can be from a feature that I am machining zero verses the part zero. With G54.2 or G54.4 you now have the ability to fine tune a specific details without needing to have 100’s of work offsets on the part. You can still go about creating 100’s of workoffsets if that is your preferred method. Now that Methods has taken over the importing of OKK machines I am not sure whom you need to speak to. I have had to go into several shops with OKK machines and help dial in the parameters to get G68.2 working correctly. Had one customer get a machine with G68.2 and never use it. Then crashed their machine and started having quality issues with their parts. Since it was such a bad crash it was impossible to get the kinematics back to factory specs. The machine builder begged them to try G68.2 to show them if they used them in the machine correctly they could make good parts again. Since it was already built into the post they just had to make the change and do a little implementation work and they were back to holding .0002” tolerances on their parts like they were before the crash. Sorry for the lengthy response no power so just killing time on my IPad. Have a good day.

"C:\Program Files\Mastercam 2020\Mastercam\documentation\en-US\Quick_Ref_Card.pdf" theres also a shortcut to it in your Start Menu in the Mastercam Folder

Make sure your custom tooling is set to a level that will never be used by anything else. Our custom tooling starts at level 8001and ends at 10000. We're currently at 8630ish so we still have growing room.

If you use an Optirough path you can select the boss as a separate "Machining Geometry" set, from the faces you've chosen as your 1st Machining Geometry set. Then you can set the distance away from the boss that you wish.

You did a pretty good job getting to the point you have gotten. Thank you for sharing a file with sweat equity in it. I would use the same process you used on OP7 in the Index Plane to finish roughing out the ID area. Make a Boundary to allow for your tool to start in the empty space. I normally will make it 2X to 3X larger than my tool. One other thing name your operations as your making them. Hard to follow what your doing without clicking each operation to see it. I did an 1800 part and every single operation was labeled. Looks like PHD designed this part with the .125R in one place and then 0.134375 in others. I would still use a 3/8 x .125R to swaff the walls after you get the meat out. You have a .0625R in the top 2 pads and can 3+2 then using your plane or you can 5 Axis them using Swarf. You have about 1/2 hour to one hour of programming left and it is done ready to flip. I would make a set of jaws to ID grab the part then finish the outside with a flat ground bottom endmill. Not a flat endmill, but a Flat Ground Endmill. Most endill have a slight taper in the cneter and will not flat cut correctly and leave scallops on your surface. A good flat ground bottom endmill will make that thing look like new money. You can use 5 axis Parrella with surface and call it a day on the side walls and round outside. Then come back with a nice 1/2 ball endmill to clean up the radius. Could get a Radius mill the 0.2343R, but then have to worry about blending it. Define your holders. Not defining holders is sloppy in my opinion. You also have some crashes your not seeing by not defining you holders. Define your work holding plenty of free models out there from just about anyone. Put some of this to effort and come back trying to do more and we will help you along more. Here is a Video of the 5Axis Finish Video