5-axis positioning using fixture offsets

To do 5-axis positioning using fixture offsets:

1. Create a part with multiple Setups.
2. On the Indexing tab of the Stock Properties dialog, select 5th Axis Positioning and click Fixture Location.
3. Set the Offset of Touch-off Point from Machine Zero.
4. For the First Axis Rotational Offset, enter the angle (measured counter-clockwise) between the spindle and the A-axis when the B angle is set to 0. For example, the A-axis faces the spindle when B is set to 0, then enter 0. If it faces the door when B is set to 0, then enter -90. This offset will be set the same for all parts machined on a specific machine.
5. Click OK to close the 5 Axis Fixture Location dialog.
6. Select the dominance from:
   • Tool Dominant — If you want the order of operations to be tool dominant across all Setups, select this option.
     Note: You must also select Minimize tool changes in the Automatic ordering options dialog for Tool Dominant to work correctly.
   • Setup Dominant — If you want the order of operations to complete each Setup before moving on to another Setup, select this option. The milling ordering attributes determine the order in which operations are performed within a Setup.

     Select Generate Single Program if you want to create a single 5-axis indexed program. When this option is selected, you need only specify the simulation information for the first setup and it is used for all setups.

7. Click OK to close the Stock Properties dialog.
8. Generate toolpaths. Enable Minimize tool changes if you want tool-dominant toolpaths.

   The simulation works for both centerline and 3D simulation. In centerline simulation an arc is displayed for a 5-axis reorientation. In 3D simulation the part position and orientation stays fixed and the tool moves. The tool does not move smoothly between Setups, it simply reappears in the new Setup.

9. Select a post processor that supports fixture offsets and create NC code.
10. The NC code is generated relative to the coordinate system of each Setup. If you want to see the NC code for each Setup specified in machining coordinates (Y up and X to the right), then each Setup should be positioned so that the Setup coordinate system is aligned with the machine coordinates when that face is pointing toward the tool. The operator must touch-off each Setup individually.