NC Code Format for Threading Operations
The NC code format determines how stock is removed when machining a thread in Mastercam Lathe. It also determines how much flexibility you want in setting the amount of stock to be removed per pass. The G-code that displays in the NC file depends upon the format you choose. NC code formats are described below.
- Canned: Generates one or two lines of NC code for the entire toolpath. The machine control calculates how much area needs to be removed to create the thread and removes this area in equal amounts per pass. If you select this option, you can edit only the cutting depth of the first cut. The post processor code is G76 for most machine controls.
- Longhand: Generates one or more lines of NC code for every pass that the tool takes to create the thread. The post processor code is G32 for most machine controls.
- Box: Choosing this option is similar to longhand in that it generates one or more lines of NC code for every pass that the tool takes to create the thread. With box threading however, the tool in-feed direction is perpendicular to the axis of the thread. The post processor code is G92 for most machine controls.
- Alternating: Choosing this option is similar to longhand in that it generates one or more lines of NC code for every pass that the tool takes to create the thread. The in-feed moves are computed so that the side of the insert making the cut is reversed on every pass. For example, with the first pass the left side of the insert makes the cut and with the second pass the right side of the insert makes the cut, etc. The post processor code is G32 for most machine controls.
Your control must be capable of supporting the NC format that you choose. Use the Lathe Canned Cycles section of the control definition to tell Mastercam how your control supports thread toolpaths. Some post processors require you to use Miscellaneous Values to define a chamfer.





