To Create a Curve Cut Motion
1. On the Trajectory tab, click Tool Motions.
2. Select Curve Cut from the Tool Motions list. The Curve Cut dialog box opens.
This dialog box has the References tab that enables you to create a curve trajectory and the Axis Control tab that enables you to add tool axis definitions. The following steps are applicable only to the References tab.
3. In the Trajectory Curve collector, specify the curve cut along which, the cut motion should be created.
4. To remove the selected curve, right-click the curve in the Trajectory Curve collector and click Remove.
5. Click Details to open the Chains dialog box and specify a chain of curves that collectively form the trajectory.
The ends of an open-ended chain are displayed as draggers. You can trim and extend the chain by selecting the dragger in the graphics window and subsequently selecting Extend To and Trim At from the shortcut menu. You can also type the values for start and end point of the chain in the graphics window
6. For closed loops the origin of the loop is displayed as a dragger. You can move this dragger to any location on the chain to set the start point for the curve cut.
Alternatively, click Start Point to change the location of the start point. For details see, Start Point for Closed Loops in Trajectory Milling.
7. Select Helical Cut to create a helical cut motion with a start or end depth from a surface. The parameters HELICAL_RAMP_ANGLE , HELCIAL_PITCH, HELCIAL_BOUNDS, and ADJUST_PITCH can be used in helical toolpath generation. For details on these parameters, see topic Milling Parameters.
If you convert a 3- axis trajectory step with a helical cut to a 4- or 5- axis step, the curve cut motion switches to the standard multiple cut behavior.
Helical cut is not supported for 4- and 5- axis curve cuts.
8. In the Start Height collector, specify the reference plane or surface that defines the depth of the first pass.
9. In the Height collector, specify a reference plane or surface that defines the depth of the cut motion.
10. To remove the reference plane or surface, right-click the reference plane or surface in the Height collector or the Start Height collector and click Remove.
11. SelectOffset Cut to offset the tool from the reference by an offset distance. The offset distance is half of the CUTTER_DIAM value. The direction of the offset is with respect to direction of trajectory.
12. Click to flip the material removal side or offset direction from one side of the cut to the other.
The direction arrow is displayed on the chain. You can click the arrow to change the direction. Alternatively, in the Chain dialog box that opens when you click Details, click Flip on the Options tab to change the direction.
13. Define the parts and surfaces that can be used as a limit on the tool motions during machining. Use any of the following options in the Check Surfaces section:
Add Reference Parts—Adds the reference parts used in the assembly to the collector.
Use Mill Stock Allowance—Specifies that mill stock allowances will be used to keep a safe distance from the check surfaces. This distance is the same as the stock allowance for machined surfaces.
If you do not specify the mill stock allowance, the CHECK_SRF_STOCK_ALLOW parameter is applied by default.
Check Surfaces Collector—Specifies parts and surfaces the cutting tool checks against during tool path computation. The tool path is trimmed automatically to not violate these surfaces and to consider any stock allowance you have defined.
Details—Opens the Surface Sets dialog box that allows you to specify the surfaces to be considered for gouge checking. For more information, see To Select Surfaces.
14. Click to save the changes and close the Curve Cut dialog box or click to cancel the definition of the curve trajectory.