NX Rough Plunging a Turning Groove with a Single Pass on the Center of the Groove

Two tools will be used to cut a groove on a Turning part. The first tool will be used to rough by plunging the tool on the center of the groove. The second will be used to finish. Using two tools will help to improve the accuracy and the surface finish. This article will help to explain how to create the center roughing pass.

1. Verify that Main -> Strategy -> Plunge Alternate and that Main -> Cleanup -> None are set.

2. Set Strategy -> Minimum Cut Depth -> Specify  to a value larger than the possible step over. Entering a large enough value is important for getting a single cut pass.

3. The Corners -> Normal Corners and Corners -> Shallow Corners  options can be set to Extend to remove extra tool motion.

4. The Chip Control option can be enabled to break the chip when plunging.

5. Pick Non Cutting Moves -> Approach -> Motion to Start of Engage -> Clear Radial -> Direct.

6. Set Non Cutting Moves -> Departure -> Motion to Return Point -> Clear Radial -> Direct.

7. Specify the Stock, Tol.& Clearance -> Clearance Planes -> Radial Limit Option to define the clearance plane

8. Use Options -> All other Parameters -> Region Machining -> Multiple if more than one Cut Region is turned.

9.  Optionally, Trim Planes can be used to contain the cut. Two Radial and two Axial Trim Planes are used in the picture below.

10. It may be necessary to cut the two grooves in separate operations depending on the geometry of the part.

Notes