Manufacturing > Milling > General Information > To Customize the Tool Path in Milling
To Customize the Tool Path in Milling
Generally, the system automatically generates a default tool path based on the cut geometry and manufacturing parameters. For more low-level control over the tool path, you can use the Customize option in the NC SEQUENCE menu.
For all Milling NC sequence types, except Trajectory Milling, the system automatically generates an Auto Plunge and the default Automatic Cut motion. You can either accept the motions automatically generated by the system (and supplement them with the Approach and Exit Tool Motions, if needed), or delete them and generate your own Automatic Cut motions, as well as Approach and Exit Tool Motions. For Trajectory Milling, cut geometry is not specified at the time of NC sequence setup; you have to use the Customize functionality to generate the Automatic Cut, Approach, and Exit Tool Motions.
Build Cut at the NC Sequence Level
When you create Automatic Cut motions, the Build Cut functionality lets you add or remove slices or cutting passes, specify approach and exit path, and so on. However, if you are satisfied with the default tool path generated by the system (which is based on the sequence parameters and geometric references), you can use the Build Cut option in the SEQ SETUP menu to access the Build Cut functionality at the NC sequence level, without having to go through the Customize user interface.
This option is available only if the NC sequence’s tool path has not been customized. If you define Build Cut items at the NC sequence level, and then attempt to customize the tool path, the system prompts you first to delete the items defined at the NC sequence level. An Info Window opens with a list of items you must delete. The Build Cut functionality at the NC sequence level is available for Volume, Local, Surface milling, Face milling, and Pocketing.
The Build Cut functionality at the NC sequence level is identical to that at the Automatic Cut motion level.
The Build Cut option allows you to specify approach and exit motions or entry point for the cut motion. When you select Approach or Exit, the following options are available:
Point—Create or select an axis to be used as a start (end) point. The axis can belong either to the workpiece or to the design model, and must be normal to the retract plane. The approach (exit) path will lie at the depth of the start (end) of the cut motion.
Sketch—Sketch the approach (exit) path for the tool in the XY-plane of the Operation coordinate system. The path will lie at the retract plane level. The tool will plunge at the end of the approach path and move in a straight horizontal line to the start of the cut motion. At the end of the cut motion, the tool will move in a straight horizontal line to the start of the sketched exit path, retract to the retract plane level, and follow the exit motion. Use the Tool Motion functionality to specify other types of approach and exit motions.
Each Slice—Apply the approach (exit) instructions to each slice of the tool path.
First Slice—Apply the approach instructions only to the first slice of the tool path.
Last Slice—Apply the exit instructions only to the last slice of the tool path.
The Entry Point option allows you to select the corner to start machining from. The corners available as an entry point are displayed, with one of them highlighted. Select the corner desired using Next, Previous, and Accept.
Use the Delete and Redefine commands to cancel or change the approach or exit instructions. The Play Cut command displays the tool path.