First let me talk about Rule #1. Anytime you have a G0 (Rapid) function, the Z-Axis MUST be at the Clearance or Safe Plane so that it doesn’t hit (A) your clamps, (B) Your vise, or © surfaces on your part that are higher than Z0 (Often found on 2nd operation machining)
Next, let me see if I can paint this scenario in your mind.
Scenario (1) I have a piece of hex bar sitting in a vise. I want to machine both ends or the rod. The Home location (XYZ 0) is the center/end on one side of the rod. If my machine is sitting at XYZ home, and the first end to be machined is opposite of the home end, and I used the Carbide3D post, the machine will (try) to GO Rapid THROUGH my part because it didn’t raise the Z-Axis to the Clearance Plane first = CRASH
Scenario (2) I have a 6 x 6 flat plate that is set up for its second operation. I will C’Bore several holes. There is a single clamp in the middle of the plate holding it to my table. XY0 is the Center of one of the holes, and Z0 the top surface near on of the holes. I have used the Carbide3D Post, and press Run. The machine then rapids to the first hole to be machines and tried to rapid right THROUGH the clamp because it didn’t raise the Z-Axis to the Clearance Plane first and CRASH
Yes, I could have taken the time to see which end OR hole was machines first, but a GOOD POST takes care of the operator and ALWAYS rapids at a safe Clearance plane, and that is why I wrote a GOOD (new) Post.
I also understand that 99% of the Shapeoko users out there are not at the level of machining that I am and that the Carbide3D post works just fine, and I am ok with that, but I am NOT ok that it rapids unsafely, and that someday it will bite you in the ass, (because it’s not fool proof post)
PS I love the Post Processor in Carbide Create in that it allows you to set the Z Clearance height (Default is 12mm, and my clamps are 12.7 mm, yeah, I now have a clamp with a 0.7 rapid mill grove through it…lessen learned, new Z height 25mm). It’s a good post.
You had a lot of question, and I think I answered them all, but if I didn’t please let me know.