Work Offset Numbers

There are many places in Mastercam where you can enter a work offset number so that a particular work offset is applied when a toolpath is created or modified. For example, you can associate a work offset with a plane so that it is used whenever the plane is selected, or you can enter a work offset as part of the operation parameters for an individual toolpath.

Many users associate work offsets with specific G-codes, most commonly G54, G55, etc. However, because different machine tools and controls use many different offset numbering schemes, Mastercam requires that you specify work offsets in a generic format. Offsets are identified starting with the number zero and increment by one for each successive offset. For example, in Fanuc controls, 0=G54, 1=G55, 2=G56, etc., while in Fadal controls 0=E1, 1=E2, and 2=E3. Your post processor should be configured to output the proper codes when you post the operation. The NCI file will contain the generic codes.

The Automatic setting enables automatic work offset incrementing. This feature increments the work offset value by one, every time there is a tool plane rotation. This feature is typically used with a Milling machine that has a rotary axis. For example, if you use 3-axis Fanuc VMC and you create four tool planes that rotate around the X-axis, all with a work offset setting of Automatic, you would get G54, G55, G56, and G57, respectively. You can set a work offset value in the toolpath parameters, or by assigning a work offset value to every tool plane.

When you enter a work offset as part of the operation parameters, it overrides an offset that has been set elsewhere. For example, if a work offset has been set because it is associated with a plane that has been selected, you can override it by selecting a new work offset in the toolpath parameters.

Use the Work System page in Control Definition to tell Mastercam more about your work offset scheme.

Learn more