To Create a GoTo Point Motion
GoTo Point motions enable the tool to go to any datum point (not just a control point). You can restrict moves along some of the axes of the NC sequence coordinate system. For 4- and 5-Axis NC sequences, you can also change the tool axis orientation.
1. ClickGoTo Point in the list in the Customize dialog box, and click Insert. The Goto Point dialog box opens.
2. In the Tip# box, select the tool tip that you want to use to reach the datum point.
3. Edit the Tool Motion parameters, if desired, using the Feed, Spindle, and Coolant buttons in the top portion of the box.
4. Click Specify Point to create or select the control point. The CR/SEL POINT menu opens with the options:
◦ Select—Select an existing control point or datum point.
◦ Create—Create a new control point or datum point:
On Toolpath—Create a new control point by selecting on the tool path.
Datum Point—Create a new datum point using the regular functionality for creating datum points. The datum point will belong to the workpiece in Part machining, and to the manufacturing assembly in Assembly machining.
The Specify Offset button allows you to specify a target point offset from the control point created using the Specify Point button, described above.
5. Do any of the following in the next portion of the dialog box to restrict moves along some of the axes of the NC Sequence coordinate system:
◦ If the Simultaneous option button is selected, then, depending on whether the X Axis, Y Axis, or Z Axis checkbox is selected or unselected, 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. For Turning, only the X Axis and Z Axis buttons will appear in the dialog box.
◦ If the Z First option button is selected, 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 (for Turning, this is the X-axis; for other types of NC sequences, this is the XY plane).
◦ If the Z Last option button is selected, the tool moves along the X-axis (for Turning), or in the XY plane (for other types of NC sequences), from the current position to the location of the selected point, and then moves along the Z-axis to arrive at selected point.
6. If you want to define a 4- or 5-Axis NC sequence, you can also change the tool axis orientation at target point:
◦ Along Z Axis—Use the default orientation of the tool (parallel to the Z-axis of the NC Sequence coordinate system).
◦ Use Previous—Use the previous tool orientation.
◦ Specify New Axis—Click Specify Axis and select an edge or axis that the tool axis will be parallel to, or a surface that the tool axis will be normal to. Finalize the tool orientation using Flip and Okay options; note that the red arrow must point from the tool tip towards the toolholder.
7. The Preview button allows you to preview the tool motion defined. Click OK if satisfied or Cancelto quit creating the tool motion.