This is how simple the programming on these machines can be.
Press the MDI (manual data input) button and the screen in the background appears.
Line 0000 is already there, it is a date and time stamp
Line 0010 Is the tool change call
Line 0020 is optional, I put a rapid move in well outside of the part because otherwise it will rapid right to the start position and I do not like that
Line 0030 is optional, a program stop which stops it at the first move, this is a personal choice.
Line 0040 is the thread cycle which opens the screen in the foreground
The actual G-Code is generated by the control and may be easily viewed and edited if required. There are certain operations that the software will not run in this mode, such work requires CAM or Fingercad.
Enter 1 for for OD threads
Enter the lead 4 TPI = .25
Enter the thread Depth, I used the MH thread data
Enter the Doc of the first pass
Enter the DOC of all but the last 2 finish passes
Enter the DOC of the finish passed
Enter the number of spring passes
Enter the distance that the tool moves outside the major diameter
Enter the angle at which the tool approaches the work, I do not believe that this is important but that is a point of much angst for many hobbyists
Enter the Z position where the thread starts, in this case it is a straight thread so the thread began .200" before Z 000, if a tapered thread start at 000
Enter the End Z position where the thread ends in the undercut
Enter the start diameter, this will be smaller then the end diameter with a tapered pipe thread
Enter the end diameter
Press enter and thread away.
This assumes that you know enough that you have already turned the stock to size, chosen the tooling and set it, prepared the work holding, order of operations, compiled the thread data and chosen a spindle speed.
It merely takes the drudgery out of repetitive operations such as this, anyone that is proficient at running a manual lathe would be knocking out parts in one day.