External and internal machining, commonly known as turning and boring, are the most common operations on CNC lathes. Either operation involves roughing and finishing toolpaths and can range from very simple to very complex. Roughing means removal of a significant portion of the material and forming the shape that will be finalized during finishing. Multiple repetitive cycles G70, G71, G72 and - a to a much smaller extent - G73, are very useful for this type of work. Depending on the job setup and complexity, the CNC programmer has to deal with many issues that relate to roughing and finishing, with or without using multiple repetitive cycles. This chapter describes various techniques that can be used in many turning and boring operations on CNC lathes.

Selecting program zero (part zero) for lathe parts is always related to the Z-axis. Without an exception, the program zero for the X-axis must be the spindle centerline. When it comes to the Z-axis zero selection, there are several methods that may at least be evaluated and either rejected or accepted. The illustration at right shows five reasonable options, identified by a reference letter. The Z-zero position can be anywhere, but there is some credibility in the five options.

• Position A - Front face of the stock

Although this face is easy to reach during tool setup, selecting the stock front face has several disadvantages. First one is that the stock will be removed by facing in the early stages of machining, but the amount removed will have to be included in all absolute Z-axis motions. The second disadvantage is that the stock amount is not always consistent.

• Position B - Front face of the part

This is the most popular overall selection, and for a good reason. Many, if not all, dimensions on the drawing originate front the front face and can be used directly. Another advantage is that all Z-axis dimensions in the drawing will be negative - forgetting the minus sign in the program will force the cutting tool away from the part. Setup using the touch-off method is not difficult.

• Position C - Back face of the part

This is probably the least favorable location from the five possibilities listed. It is hard to measure and provides virtually no benefits, even if some drawing dimensions originated from this face. Keep in mind that when the part is turned around, this will be the preferred face - see Position B .

• Position D - Jaws face

In some cases, this is face may be the rough stock, in other it may be the finished back face. Face of jaws is easy to measure and may benefit some castings or forgings where the stock length varies. On the negative side, the remaining rough stock must be always accounted for, if present.

• Position E - Chuck face

Unless the chuck is replaced, the chuck face remains the same for any job. No other benefits.