Hole pocketing operation can be split up into 3 outputs
1.Circular interpolation (this is output when you select clean up pass at each Z level)
2.Helical interpolation (this uses the helix parameters defined under the entry/exit tab)
On most machines, helical interpolation is output as G02/G03 X Y Z I J (each helix is output as a separate line of G02/G03 code and the Z represents the helix pitch)
Make sure to select Output full 360 helix and each helix individually
3.Spiral Interpolation (this is the toolpath that performs the XY cut between the helix to the clean up pass.)
The output for a spiral interpolation would typically be as follows: G02/G03 X Y Z I J Q. Where Q represents the spiral lead. Some machine controllers would require Spiral Start & end Radius / Spiral number of revolutions / Spiral Total Length / Spiral Angle in place of spiral lead.
Your post is currently not set up to output spiral interpolation as we are not sure if your controller supports spiral interpolation. Please check the controller documentation and send us the information with an example for a spiral output.
Go to CAM Preferences -> Output Control located on the machining operations browser. For older versions this would be under Machining Preferences.
* Check output spirals as linear motion as checked.
* Uncheck Output Arcs as Linear segments
* Uncheck output helix motions as linear segments.
Regenerate the toolpath when a change is made to machining preferences before post processing.
Make sure the post processor is configured to output helical interpolation. This is typically defined under the Helix/Spiral section in the post processor generator.