Yeah thanks, that confused me even more LOL. I'll reread what you said. I was doing 5IPM because I was engraving with a fine bit.
So I have my parts center as the center so it should be going to like 1.2" up and cutting but it doesn't do much. I'll mess with the settings.
Greg has you on the right track. Here in a nutshell is what’s required.
In Config> General Config be sure ‘Rot 360 Rollover’ is NOT checked. (Your code uses both pos and neg A values).
In Config> ToolPath select the ‘X-axes’ button; check ‘A-Rotations Enabled’ and check ‘Use Diameter for Feedrate’.
On the Settings page you have a choice with the ‘Rotation Diameter’ DRO. Unfortunately due to a problem within Mach, neither is accurate, but in your case one is better than the other.
If you enter 0.0001 in the DRO then Mach will read all Z values as a diameter and calculate the feed rate accordingly. Obviously, this is incorrect as the Z is actually a radius. The angular component of your X-A move will be off by a factor of 2. Probably not acceptable.
If you enter the Z value that is in the first block containing a Z then in this case (and in this case only) Mach will correctly use this value as a radius. However changes in Z will be incorrectly interpreted as a change in diameter thus creating another error. But this error is less and in fact wouldn’t even be noticeable if your Z clearance height were reduced. (Less change in Z; less error). Is there a reason that you need over an inch of Z clearance? (I normally use something more in the order of 0.050).
Another thing, your code uses only G01 (no G00), although it does increase the feed from F5 to F20 for the rapids. You may find it more convenient to use G00 for the rapids and thus only have to set the Feed rate once at the beginning. Easier to make changes.
Is it just me, or are you engraving a mirror image?
Hope this helps,
Al