As long as the Rotary Direction and Rotary Axis variables are set correctly, and the Machine Base Matrix is setup correctly, then the likely culprit would be the way you have your Planes setup inside Mastercam. For A(C) on B, you should have something like: #Primary axis angle description (in machine base terms) #With nutating (mtype 3-5) the nutating axis must be the XY plane rotaxis1$ = vecy #Zero rotdir1$ = -vecx #Direction #Secondary axis angle description (in machine base terms) #With nutating (mtype 3-5) the nutating axis and this plane normal #are aligned to calculate the secondary angle rotaxis2$ = vecz #Zero rotdir2$ = -vecx #Direction If you look at the Primary values (vecy and vecx), you'll notice there is no "Z" in the plane being described. This means rotation happens "Around Z" (as it should, regardless of what you label the axis address letter.) If you look at the Secondary values (vecz and vecx), you'll notice there is no "Y" in the plane being described. This means rotation happens "Around Y" for the secondary. And should be labeled "B". If the rotations happen "Backwards", in other words, you are getting "-90.", instead of "90.", all you should have to do is reverse the "sign" of the RotDir variables. (add a minus sign, or remove the minus sign. That's it.) 'mtype' should be set to '0.' Also, and this is important(!), make sure these are both set to Zero, when you are setting up the rotation angles in the Post: pang_output : 0 #Angle output options, primary sang_output : 0 #Angle output options, secondary #0 = Normal angle output #1 = Signed absolute output, 0 - 360 #2 = Implied shortest direction absolute output, 0 - 360

I mean, that's only 13:1, Depth to Diameter, on the finished feature. Piece of cake, right? That would be a difficult slot, in Aluminum. In Inconel 718? oof... I'm with Peter, I would drill out as much of that material as possible, without letting the holes intersect. Then I'd look at getting a .047 diameter endmill, from Harvey Tool, and have them relieve the neck. I would get at least 3 different lengths of tools to finish the slot. If you try to go with a single "length" to rough and finish, you'll be there for days. I'd go with a 5X (.250 to shoulder), and a 10x (.480 to shoulder), and get an additional 10x cutter, that is ground back to .658 to the shoulder. ( 14:1, D2D, on a .047 endmill) I'd look to finish with at least a couple different lengths of tool. For the bottom of the slot, I'd try a 1 mm diameter, with 1 mm length of cut, and 17:1 D2D. You could try something like a 1.25 mm diameter (.051), and try to interpolate a slot that is .0004-.0008 wide, to stay under your .055 width tolerance, but what a pain. You'd be far better served by drilling out as much material as possible, and just sending it off to get burnt out on the EDM. As slow as EDM is, you will get the part finished much faster than trying to dial in a slotting process with multiple tools that are extended way beyond the practical limit.

What machine? On mills: G84 is output (by default) for tapping, when you select the "Tap" cycle in the "drill parameters" page. G84 typically uses a "floating tap head", which allows a tiny bit of axial "float". This is used when the machine reverses the spindle at the bottom of the hole. More modern machines use a function called "Rigid Tapping", where the spindle rotation uses an encoder (and orients, typically with M19) to track the rotation position of the spindle, and the machine synchronizes the Z-Axis motion, so that it will tap successfully with a rigidly mounted tap. Many machines will have different codes to indicate "rigid tapping" vs. "non-rigid tapping". For example, G84 for non-rigid (standard), or G84.2 for Rigid Tap. Some machines have the same "G84" canned cycle call, but precede the G84 G-Code line, with M29 and the Spindle Speed for the tap. For example: M29 S350 In all cases, you must synchronize the Spindle Speed (RPM) with the Feed value. However, there are two ways to do this: Your machine can be in Feed per minute (Inches per Minute on an Inch Machine [G20], or Millimeters per Minute on a Metric machine [G21]). Feed per minute is typically indicated with G94. When you are in Feed per minute mode, the Feed value will always be: Thread Pitch x RPM. The calculation for Thread Pitch is 1 / # of Thread Per Inch. If you are in Feed per Revolution mode, then your "Feed value" may be specified as "E", instead of "F", or it may remain "F", but the value will always "equal the pitch of the thread". Because you are in G95 mode, you get better ability to adjust the actual cutting speed, because all you are doing is modifying the RPM value. Since RPM is always an integer value on machines, Feed per Revolution gives you the easiest ability to adjust to a "true pitch" value. Be careful when using Feed per Minute, as you can pick combinations of Feed and RPM, where the Feed value is "rounded or truncated", because the number of digits of precision allows for the "F" value, is not precise enough to give an accurate feed value. Example: Pitch of .08333333, where the F value is rounded to 3 decimal places (.083) is not an accurate pitch value. Where possible, I increase the F output to 4, 5, or even 6 decimal places, if the machine allows it.

You say mirrored, but I think what your really saying is the helical cuts are inversed. I tried messing with the MMD and Post to get that changed and nothing worked. I would then mirror your part along the X axis and drive the toolpaths that way. Cheat the model to get you what you need. Not ideal, but sometimes that is what you need to do to get a job done in the real world so it will be a good teaching exercise on how to think out of the box to solve the problem. Here is the file with what I was referring too. Hopefully this helps get you and the students going in the direction you all need to get what your after done. Secondary Helix 30 DEG 0.625 2019 Rev A

Damn....finally one i can answer and I'm 4 minutes too late!