To Create a Goto Point Tool Motion
With the GoTo Point motions, the tool goes to any datum point from the end of a previous motion. You can restrict moves along some of the axes of the NC sequence coordinate system.
1. On the Trajectory, Face, Profile, Manual Cycle tab, or the tab of any turning or holemaking step, select GoTo Point in the Tool Motions list. The Goto Point dialog box opens.
2. Create or select the datum point. You can select an existing datum point or perform the following actions:
◦ Create a datum point. The datum point belongs to the workpiece in Part machining, and to the manufacturing assembly in Assembly machining.
3. Use the Offset options to specify a target point offset from the point created as described above. You can specify offsets along the X-, Y-, and Z- directions.
4. You can restrict moves along some of the axes of the NC Sequence coordinate system using the following options:
◦ If you select Simultaneous, then depending on whether you select or clear the X Axis, Y Axis, or Z Axis check box, the tool is allowed or disallowed to move along this axis. By default, all the axes are allowed. The tool then moves directly from the current position to the target point. If some of the axes are disallowed, the final tool position is computed based on the current point and the axes allowed.
◦ If you select Z First, the tool moves along the Z-axis from the current position to the level of target point; it then moves using all remaining available axes to the target point.
◦ If you select Z Last, the tool moves along the X-axis, or in the XY plane for other types of NC sequences, from the current position to the location of the selected point. It then moves along the Z-axis to arrive at selected point.
5. Click Parameters to edit the Tool motion parameters.
6. Click OK to create the Goto Point motion, or Cancel to cancel.