Manufacturing > Milling > Local Milling > To Create a Local Milling NC Sequence by Pencil Tracing
To Create a Local Milling NC Sequence by Pencil Tracing
1. Ensure that the active operation references a Mill/Turn workcell.
2. Click Mill > Milling > Pencil Tracing. The SEQ SETUP menu appears.
3. The following local milling specific commands are available on the SEQ SETUP menu in addition to the common commands for all NC sequence types:
—Select the type of cutting tool. The following types of tools are supported:
End Mill
Ball Mill
Bull Mill
Taper Mill
Prev Tool
—Select the previous larger tool cutting tool used to trace the remainder areas. The following types of previous tools are supported:
End Mill
Ball Mill
Bull Mill
* The Prev Tool option is available when you set the RESTPASS_ENABLE parameter to YES.
Retract Surf
Define a retract plane normal to the Z-axis of the orientation coordinate system. The following retract parameters are available:
—The cutting tool takes a direct route from one pass to another clearing the surface and adding a curve to speed progress. The minimum height of the retract movement is controlled by the CLEAR_BY parameter, and the shape is controlled by the CURL_DOWN_RADIUS and CURL_OVER_RADIUS parameters.
—The cutting tool only retracts vertically to the minimum the Z-height needed to clear the surface, moves along this plane in a straight line, and drops down vertically to the start of the next pass. The minimum height of the retract is controlled by the CLEAR_BY parameter.
Surfaces—Select surfaces to be milled during this NC sequence.
Window—Create or select a Mill Window. This option and Surfaces are mutually exclusive. If you use the Window option, then all the surfaces within the specified Mill Window will be selected.
Build Cut—Access the Build Cut functionality.
The required options are checked off automatically. Select additional options, if desired, and click Done. The system will start the user interface for all selected options in turn.
4. On the NC SEQUENCE menu, click Play Path to verify the tool path automatically generated by the system. If not satisfied, you can either modify the parameters, or use the Customize functionality to adjust the tool path.
5. Click Done Seq or Next Seq when satisfied.