But why does it make the little cut right before the chamfer.
Hello cuttergrinder,
The issue with the Step at the front end of the parts has Zero to do with TNR Compensation. I suspect that its caused by:
1. The Z Workshift is incorrectly set for the Workpiece
or
2. The Geometry, or Wear Offset for the tool being used is incorrect.
In the following picture, I believe that the features that are indicated with Coordinates will correspond to your actual Workpiece.
You can Check this out via MDI by calling the Tool with its Offset and move the tool by Hand-wheel to touch the end of the Workpiece; observing the Absolute Z coordinate display will tell you where the end of the Workpiece is. Further, if you touch the Tool on the Z surface that is cut, the Absolute Z display should show a value equal to the Z Finish Allowance set in the 2nd G71 Block.
When using a Tool Set as a Type 3 Tool (providing it actually is a Type 3 Tool), then the True Tool location when cutting surfaces that are parallel to the respective X or Z axis, is the same whether TNR Comp is used or not. Accordingly, check the Offset setting for the Tool involved, and the Workshift Offset.
Many Fanuc Control Models ignore TNR Comp completely in G71. If TNR Comp is used in the G71 profile definition it will be correctly executed when the G70 cycle is run. The only Fanuc models that it could be consistently said that TNR Comp in G71 was a feature are FS10, 11 and 12 controls and was well documented in the Fanuc Manual.
Regards,
Bill